Abaqus > Building A Model > Element Properties
XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">   
Element Properties
By choosing the Element Properties item, located on the application switch for Patran, an element properties form will appear. When creating element properties, several option menus are available. The selections made in these option menus will determine which element property form is presented, and ultimately, which ABAQUS element will be created.
The following pages give an introduction to the Element Properties form, followed by the details of all the element property definitions supported by the Patran ABAQUS Application Preference.
Element Properties Form
When Element Properties is selected on the main menu, this is the form which will be displayed. Four option menus on this form are used to determine which ABAQUS element types are to be created, and which property forms are to be displayed. The individual property forms are documented later in this section. For more details, see the Element Properties Forms (p. 61) in the Patran Reference Manual.
The following table shows the allowable selections for all option menus when Analysis Type is set to Structural.
Dimension
Type
Option 1
Option 2
Name
0D
Mass
 
 
MASS
 
 
ROTARYI
Grounded Spring
Linear
 
SPRING1
SPRING2
Grounded Damper
Linear
 
DASHPOT1
DASHPOT2
IRS (single node)
Planar
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping
No Separation
Lagrange Vis Damping
Lagrange Vis Damping No
Separation
IRS12
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No Separation
Lagrange Vis Damping
Lagrange Vis Damping No
Separation
IRS13
1D
Beam in XY Plane
Standard Formulation
Hybrid
Cubic Interpolation
Cubic Hybrid
B21, B22
B21H, B22H
B23
B23H
 
 
Standard Formulation
Hybrid
Cubic Interpolation
Cubic Hybrid
B21, B22
B21H, B22H
B23
B23H
 
 
Standard Formulation
Hybrid
Cubic Interpolation
Cubic Hybrid
B21, B22
B21H, B22H
B23
B23H
 
 
Standard Formulation
Hybrid
Cubic Interpolation
Cubic Hybrid
B21, B22
B21H, B22H
B23
B23H
 
 
Standard Formulation
Hybrid
Cubic Interpolation
Cubic Hybrid
B21, B22
B21H, B22H
B23
B23H
 
 
Standard Formulation
Hybrid
Cubic Interpolation
Cubic Hybrid
B21, B22
B21H, B22H
B23
B23H
 
 
Standard Formulation
Hybrid
Cubic Interpolation
Cubic Hybrid
B21, B22
B21H, B22H
B23
B23H
 
 
Standard Formulation
Hybrid
Cubic Interpolation
Cubic Hybrid
B21, B22
B21H, B22H
B23
B23H
 
Beam in Space
Standard Formulation
Hybrid
Cubic Interpolation
Cubic Hybrid
Cubic Initially Straight
B31, B32
B31H, B32H
B33
B33H
B34
 
 
Standard Formulation
Hybrid
Cubic Interpolation
Cubic Hybrid
Cubic Initially Straight
B31, B32
B31H, B32H
B33
B33H
B34
 
 
Standard Formulation
Hybrid
Cubic Interpolation
Cubic Hybrid
Cubic Initially Straight
B31, B32
B31H, B32H
B33
B33H
B34
 
 
Standard Formulation
Hybrid
Cubic Interpolation
Cubic Hybrid
Cubic Initially Straight
B31, B32
B31H, B32H
B33
B33H
B34
 
 
Standard Formulation
Ovalization Only
Ovalization Only with Approximated Fourier
ELBOW31,
ELBOW32
ELBOW31B
ELBOW31C
 
 
Standard Formulation
Hybrid
Cubic Interpolation
Cubic Hybrid
Cubic Initially Straight
B31, B32
B31H, B32H
B33
B33H
B34
 
 
Standard Formulation
Hybrid
Cubic Interpolation
Cubic Hybrid
Cubic Initially Straight
B31, B32
B31H, B32H
B33
B33H
B34
Standard Formulation
Hybrid
Cubic Interpolation
Cubic Hybrid
Cubic Initially Straight
B31, B32
B31H, B32H
B33
B33H
B34
Standard Formulation
Hybrid
B31OS, B32OS
B31OSH, B32OSH
Standard Formulation
Hybrid
Cubic Interpolation
Cubic Hybrid
Cubic Initially Straight
B31, B32
B31H, B32H
B33
B33H
B34
Standard Formulation
Hybrid
Cubic Interpolation
Cubic Hybrid
Cubic Initially Straight
B31, B32
B31H, B32H
B33
B33H
B34
Standard Formulation
Hybrid
Cubic Interpolation
Cubic Hybrid
Cubic Initially Straight
B31, B32
B31H, B32H
B33
B33H
B34
Truss
Standard Formulation
Hybrid
 
CID2, CID3
CID2H, CID3H
Spring
Linear
SPRINGA
SPRING2
Nonlinear
 
Damper
Linear
DASHPOTA
DASHPOT2
Nonlinear
 
1D
(continued)
Gap
True Distance
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping
No Separation
Lagrange Vis Damping
Lagrange Vis Damping No
Separation
GAPCYL
True Distance
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping
No Separation
Lagrange Vis Damping
Lagrange Vis Damping No Separation
GAPSPHER
True Distance
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis DampingNo
Separation
Lagrange Vis Damping
Lagrange Vis Damping No
Separation
GAPUNI
Axisym Shell
 
SAX1, SAX2
1D
(continued)
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis DampingNo
Separation
Lagrange Vis Damping
Lagrange Vis Damping No Separation
 
INTER1
ISL (in plane)
Planar
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No Separation
Lagrange Vis Damping
Lagrange Vis Damping No Separation
ISL21, ISL22
 
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No
Separation
Lagrange Vis Damping
Lagrange Vis Damping No
Separation
ISL21A, ISL22A
ISL (in space)
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No Separation
Lagrange Vis Damping
Lagrange Vis Damping No Separation
ISL31, ISL32
ISL31, ISL32
1D
(continued)
ISL (in space) (continued)
Radial
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No
Separation
Lagrange Vis Damping
Lagrange Vis Damping No
Separation
ISL31A, ISL32A
 
 
 
--
IRS (planar/axisym)
Planar
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No
Separation
Lagrange Vis Damping
Lagrange Vis Damping No
Separation
IRS21, IRS22
 
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No
Separation
Lagrange Vis Damping
Lagrange Vis Damping No
Separation1D (cont.)
IRS21A, IRS22A
 
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No
Separation
Lagrange Vis Damping
Lagrange Vis Damping No Separation
 
IRS31, IRS32
1D
(continued)
 
 
--
--
--
--
R2D2, RAX2
 
Rebar
Axisymmetric
 
SFMAX1, SFMAX2
 
 
General Axisymmetric
 
SFMGAX1, SFMGAX2
 
 
 
 
 
 
ALIGN
 
 
 
 
AXIAL
 
 
 
 
BEAM
 
 
 
 
CARTESIAN
 
 
 
 
JOIN
 
 
 
 
JOINTC
 
 
 
 
LINK
 
 
 
 
ROTATION
 
 
 
 
SLOT
 
 
 
 
TRANSLATOR
 
 
 
 
WELD
 
 
 
 
 
 
 
 
ALIGN
 
 
 
 
AXIAL
 
 
 
 
BEAM
 
 
 
 
CARDAN
 
 
 
 
CARTESIAN
 
 
 
 
CONSTANT VELOCITY
 
 
 
 
CVJOINT
 
 
 
 
CYLINDRICAL
 
 
 
 
EULER
 
 
 
 
FLEXION-TORSION
 
 
 
 
HINGE
 
 
 
 
JOIN
 
 
 
 
JOINTC
 
 
 
 
LINK
 
 
 
 
PLANAR
 
 
 
 
RADIAL-THRUST
 
 
 
 
REVOLUTE
 
 
 
 
ROTATION
 
 
 
 
SLIDE-PLANE
 
 
 
 
SLOT
 
 
 
 
TRANSLATOR
 
 
 
 
UJOINT
 
 
 
 
UNIVERSAL
 
 
 
 
WELD
 
 
 
Axisymmetric Link
Gasket Behavior Model
GKAX2
 
Thickness Behavior Only
GKAX2N
 
Built-in Material
GKAX2
 
3D Link
Gasket Behavior Model
GK3D2
 
Thickness Behavior Only
GK3D2N
 
Built-in Material
GK3D2
 
2D Link
Gasket Behavior Model
GK2D2
 
Thickness Behavior Only
GK2D2N
 
Built-in Material
GK2D2
2D
Shell
Thin
Laminate
STRI35, S4R5, STRI65, S8R5, S9R5
Thick
Homogeneous
Laminate
S3R, S4R, STRI65, S8R
Homogeneous
Laminate
STRI35, S4R5, STRI65, S8R5, S9R5
Homogeneous
Laminate
S3R, S4R, STRI65, S8R
 
 
 
S3R, S4R, S8R
2D Solid
Standard Formulation
CPE3, CPE4, CPE6, CPE8
Hybrid
CPE3H, CPE4H, CPE6H, CPE8H
Hybrid / Reduced Integration
CPE4RH, CPE8RH
Reduced Integration
Incompatible Modes
Hybrid/Incompatible Modes
Modified
Modified/Hybrid
CPE4R, CPE8R
CPE4I
CPE4IH
CPE6M, CPE6MH
Standard Formulation
Reduced Integration
Incompatible Modes
Modified
Modified/Hybrid
CPS3, CPS4, CPS6, CPS8
CPS4R, CPS8R
CPS4I
CPS6M, CPS6MH
2D
(continued)
2D Solid (continued)
Standard Formulation
CAX3, CAX4, CAX6, CAX8
Hybrid
CAX3H, CAX4H, CAX6H, CAX8H
Hybrid/Reduced Integration
CAX4RH, CAX8RH
Reduced Integration
CAX4R, CAX8R
Incompatible Modes
CAX4I
Hybrid/Incompatible Modes
CAX4IH
Modified
CAX6M
Modified/Hybrid
CAX6MH
Standard Formulation
CGAX3, CGAX4, CGAX6, CGAX8
Hybrid
CGAX3H, CGAX4H, CGAX6H, CGAX8H
Hybrid/Reduced Integration
CGAX4RH, CGAX8RH
Reduced Integration
CGAX4R, CGAX8R
Standard Formulation
 
M3D3, M3D4, M3D6, M3D8, M3D9
Reduced Integration
 
M3D4R, M3D8R, M3D9R
2D Interface
Planar
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No
Separation
Lagrange Vis Damping
Lagrange Vis Damping No Separation
INTER2, INTER3
2D
(continued)
2D Solid (continued)
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No
Separation
Lagrange Vis Damping
Lagrange Vis Damping No Separation
INTER2A, INTER3A
 
IRS (shell/solid)
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No Separation
Lagrange Vis Damping
Lagrange Vis Damping No Separation
 
IRS3, IRS4, IRS9
 
 
 
--
 
 
 
R3D3, R3D4
 
2D Rebar
Cylindrical
 
SFMCL9
 
 
General
Standard Formulation
SFM3D3, SFM3D4, SFM3D6, SFM3D8
 
 
 
Reduced Integration
SFM3D4R, SFM3D8R
 
Plane Strain
Gasket Behavior Model
GKPE4
 
 
Built-in Material
GKPE4
 
 
Plane Stress
Gasket Behavior Model
GKPS4
 
 
Thickness Behavior Only
GKPS4N
 
 
Built-in Material
GKPS4
 
 
Axisymmetric
Gasket Behavior Model
GKAX4
 
 
 
Thickness Behavior Only
GKAX4N
 
 
 
Built-in Material
GKAX4
 
 
Line
Gasket Behavior Mode
GK3D4L
 
 
 
Thickness Behavior Only
GK3D4LN
 
 
 
Built-in Material
GK3D4L
3D
Solid
Standard Formulation
Laminate
 
C3D4, C3D6, C3D8, C3D10, C3D15, C3D20
 
 
Hybrid
Laminate
 
C3D4H, C3D6H, C3D8H, C3D10H, C3D15H, C3D20H
 
 
Hybrid/Red Integration Laminate
 
C3D8RH, C3D20RH
 
 
Reduced Integration Laminate
 
C3D8R, C3D20R
 
 
Incompatible Modes Laminate
 
C3D8I
 
 
Hybrid/Incomp Modes
Laminate
Modified
Modified/Hybrid
 
C3D8IH
 
C3D10M
C3D1OH
 
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No Separation
Lagrange Vis Damping
Lagrange Vis Damping No Separation
 
INTER4, INTER8, INTER9
 
Gasket
Gasket Behavior Model
 
GK3D8, GK3D6
 
Thickness Behavior Only
 
GK3D8N, GK3D6N
 
Built-in Material
 
GK3D8, GK3D6
The following table shows the allowable selections for all option menus when Analysis Type is set to Thermal.
Dimension
Type
Option 1
Option 2
Name
1D
Link
 
 
DCID2, DCID3
 
Axisymmetric Shell
 
DSAX1, DSAX2
 
 
 
DINTER1
2D
Shell
 
DS4, DS8
 
2D Solid
Planar
Standard Formulation
 
Convection/Diffusion
Convection/Diffusion with Dispersion/Control
DC2D2, DC2D4,
DC2D6, DC2D8
DCC2D4
DCC2D4D
 
 
Standard Formulation
 
Convection/Diffusion
Convection/Diffusion with Dispersion/Control
DCAX3, DCAX4,
DCAS6, DCAX8
DCCAX4
DCCAX4D
 
Planar
 
DINTER2, DINTER3
 
 
Axisymmetric
 
DINTER2A, DINTER3A
3D
Solid
Standard Formulation
 
DC3D4, DC3D6, DC3D8, DC3D10, DC3D15, DC3D20
Convection/Diffusion
DCC3D8
Convection/Diffusion with Dispersion Control
DCC3D8D
 
 
DINTER4, DINTER8
 
Point Mass
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
0D
Mass
 
 
Point/1
Options above create MASS elements with MASS properties.This creates a concentrated mass at a point. The mass is associated with the translational degrees-of-freedom at a node. The ABAQUS preference now has support for 0D (point) inertia elements using the *ELEMENT, TYPE = MASS ABAQUS input entries. With this feature you can now do a lumped mass dynamic analysis.
 
Rotary Inertia
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
0D
Rotary Inertia
 
 
Point/1
Options above createROTARI elements with ROT ARY INERTIA properties. This element allows the rotary inertia of a rigid body to be included at a node. An ORIENTATION option may also be created, as required.
Linear Spring (Grounded)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
0D
Grounded Spring
Linear
 
Point/1
Options above create SPRING1 elements with SPRING properties. This element defines a linear spring between a node and ground. An ORIENTATION option may also be created, as required.
Nonlinear Spring (Grounded)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
0D
Grounded Spring
Nonlinear
 
Point/1
Options above create SPRING1 elements with SPRING properties. This element defines a nonlinear spring between a node and ground. An ORIENTATION option may also be created, as required.
Linear Damper (Grounded)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
0D
Grounded Damper
Linear
 
Point/1
Options above create DASHPOT1 elements with DASHPOT properties. This element defines a linear damper between a node and ground. An ORIENTATION option may also be created, as required.
Nonlinear Damper (Grounded)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
0D
Grounded Damper
Nonlinear
 
Point/1
Options above create DASHPOT1 elements with DASHPOT properties. This element defines a nonlinear dashpot between a node and ground. An ORIENTATION option may also be created, as required.
 
IRS (Single Node, Planar)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
0D
IRS (single node)
Planar
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No Separation
Lagrange Vis Damping
Lagrange Vis Damping No Separation
Point/1
Options above create IRS12 elements with INTERFACE and FRICTION properties. This element defines an interface between a node on a planar model and a rigid surface.
More data input is available for creating IRS (single node, planar) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Description
Friction in Dir_1
Defines the sliding friction in the element’s 1 direction. This is the friction coefficient on the second card of the *FRICTION option definition.
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option.
Clearance Zero-Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the *SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative
Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the value on the *SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Lagrange multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
IRS (Single Node, Spatial)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
0D
IRS (single node)
Spatial
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No Separation
Lagrange Vis Damping
Lagrange Vis Damping No Separation
Point/1
Options above create IRS13 elements with INTERFACE and FRICTION properties. This element defines an interface between a node on a spatial model and a rigid surface.
More data input is available for creating IRS (single node, spatial) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Description
Friction in Dir_1
Friction in Dir_2
Defines the sliding friction in the element’s 1- and 2-directions. These are the friction coefficients on the second card of the ∗FRICTION option. If Friction in Dir_2 is specified, then the ANISOTROPIC parameter is included on the ∗FRICTION option. These values can be either real constants or references to existing field definitions.
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction
Stress
Defines the equivalent shear stress limit of the gap element. This is the equivalent shear stress limit value on the second card of the *FRICTION option.
Clearance Zero-Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the *SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative
Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the value on the *SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
General Beam in Plane
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Beam in XY Plane
General Section
Standard Formulation
Hybrid
Cubic Interpolation
Cubic Hybrid
Bar/2, Bar/3
Bar/2, Bar/3
Bar/2
Bar/2
Options above create B21, B22, B23, B21H, B22H, or B23H elements, depending on the specified options and topology. BEAM GENERAL SECTION, SECTION=GENERAL properties are also created. This defines a general section beam which is restricted to remain in the XY plane.
More data input is available for creating General Beam in Plane elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Property Name
Description
Poisson Parameter
Permits an “overall” change of the cross section dimensions as a function of the axial strains. This is the value of the POISSON parameter on the *BEAM GENERAL SECTION option.
Shear Factor
The product of this factor, the beam cross-sectional area, and the shear modulus for the material defines the transverse shear stiffness for the beam.
Box Beam in Plane/Space
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Beam in XY Plane
Box Section
Standard Formulation
Hybrid
Cubic Interpolation
Cubic Hybrid
Bar/2, Bar/3
Bar/2, Bar/3
Bar/2
Bar/2
Options above create B21, B22, B23, B21H, B22H, or B23H elements in a plane, or B31, B32, B33, B34, B31H, B32H or B33H elements in space, depending on the specified options and topology. BEAM SECTION, SECTION=BOX properties are also created. The planar box section beam is restricted to remain in the XY-plane. For the spatial beam, ∗TRANSVERSE SHEAR STIFFNESS is also created, as required.
More data input is available for creating Box Beam in Plane elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Property Name
Description
Thickness_RHS
Thickness_TOP
Thickness_LHS
Thickness_BOT
Defines the wall thickness of the element cross section. These are for the right-hand side, top, left-hand side, and bottom, respectively. These are four of the data values on the second card of the *BEAM SECTION option. These can be either real constants or references to existing field definitions. These properties are required.
Poisson Parameter
Shear Factor
Definition of XY Plane (for beams in space only)
Defines the orientation of the XY-plane of the element coordinate system. The required input is a vector in the beam’s 1-direction. This corresponds to the second line of data under the *BEAM SECTION option. All of the Patran tools are available via the select menu to define this vector.
Beam Shape Display in Plane/Space
All of the beam shapes can be displayed in their proper orientation on the 3D model. To activate the display, go to Display/Load/BC/Elem. Props... and set the "Beam Display" option. These options are discribed in detail in Display>LBC/Element Property Attributes (p. 393) in the Patran Reference Manual. The beam display is shown on beam elements only, not geometry.
Additional Beam Shapes in Plane/Space
Additional commonly used beam cross-sectional shapes are defined by forms analogous to that for box beams. The planar option defines a beam which is restricted to remain in the XY plane. For the spatial beam, *ORIENTATION and *TRANSVERSE SHEAR STIFFNESS is also created, as required.
CIRCULAR BEAM (SOLID)
This property will have the SECTION=CIRC parameter. All that is required for the definition of the cross section is the radius. The integration schemes for planar analysis (left) and spatial analysis(right) are shown below.
HEXAGONAL BEAM
This property will have the SECTION=HEX parameter. All that is required for the definition of the cross section is the circumscribing radius and the wall thickness. The integration schemes for planar analysis (left) and spatial analysis (right) are shown below.
I-SECTION
This property will have the SECTION=I parameter. The height of section, flange widths, and associated thicknesses are required. In addition, the height of the centroid, depicted as “l” is also required. This allows placement of the origin of the local cross-section axis anywhere on the symmetry line. Note also that judicious specification of the flange widths and thicknesses will allow modelling of a T-section. See p. 3.5.2-11 of the ABAQUS User’s Manual for details. The integration schemes for planar analysis (left) and spatial analysis (right) are shown below.
PIPE BEAM
This property will have the SECTION=PIPE parameter. The pipe thickness and outside radius define
the cross section. The integration schemes for planar analysis (left) and spatial analysis (right) are
shown below.
RECTANGULAR BEAM (SOLID)
This property will have the SECTION=RECT parameter. The section width and section height define the cross section. The integration schemes for planar analysis (left) and spatial analysis (right) are
shown below.
TRAPEZOID BEAM (SOLID)
This property will have the SECTION=TRAP parameter. The top and bottom width and section height define the cross section. The integration schemes for planar analysis (left) and spatial analysis (right) are shown below.
General Beam in Space
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Beam in Space
General Section
Standard Formulation
Hybrid
Cubic Interpolation
Cubic Hybrid
Cubic Initially Straight
Bar/2, Bar/3
Bar/2, Bar/3
Bar/2
Bar/2
Bar/2
Options above create B31, B32, B33, B34, B31H, B32H, or B33H elements depending on the specified options and topology. *BEAM GENERAL SECTION properties are also created. This property will have the SECTION=GENERAL parameter. *ORIENTATION and *TRANSVERSE SHEAR STIFFNESS options are also created, as required. This defines a general section beam.
 
More data input is available for creating General Beam in Space elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Property Name
Description
Area Moment I12
Defines the area moment of the element cross section. This is the I12 value on the second card of the *BEAM GENERAL SECTION option. This can be either a real constant or a reference to an existing field definition.
Torsional Constant
Defines the torsional constant of the element cross section. This is the J value on the second card of the *BEAM GENERAL SECTION option. This can be either a real constant or a reference to an existing field definition.
Definition of XY Plane
Defines the orientation of the XY plane of the element coordinate system. The required input is a vector in the beam’s 1-direction. This corresponds to the second line of data under the ∗BEAM GENERAL SECTION option. All of the Patran tools are available via the select menu to define this vector.
Centroid Coord 1
Centroid Coord 2
Defines the location of the centroid of the cross section with respect to the local cross section coordinate system. These values are either real constants or references to existing field definitions. These are the values on the ∗CENTROID suboption of the ∗BEAM GENERAL SECTION option.
Shear Centroid Coord 1
Shear Centroid Coord 2
Defines the location of the shear centroid of the cross section with respect to the nodal locations. These values are measured in the local cross section coordinate system. These values are either real constants or references to existing field definitions. These are the values on the *SHEAR CENTER suboption on the *BEAM GENERAL SECTION option.
Poisson Parameter
Shear Factor
Section Point Coord 1
Section Point Coord 2
Defines the coordinates of points in the beam cross section where output is requested. These are lists of real constants. These values are measured in the beam cross section coordinate system. The lists must have the same number of entries. These are the values on the *SECTION POINTS suboption of the *BEAM GENERAL SECTION option.
 
Arbitrary Beam in Space
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Beam in Space
Arbitrary Section
Standard Formulation
Hybrid
Cubic Interpolation
Cubic Hybrid
Cubic Initially Straight
Bar/2, Bar/3
Bar/2, Bar/3
Bar/2
Bar/2
Bar/2
Options above create B31, B32, B33, B34, B31H, B32H, or B33H elements depending on the specified options and topology. BEAM SECTION, SECTION=ARBITRARY properties are also created. ORIENTATION and TRANSVERSE SHEAR STIFFNESS options are created, as required. This defines an arbitrary section beam.
More data input is available for creating Arbitrary Beam in Space elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu
Property Name
Description
Definition of XY Plane
Defines the cross section axis N1 of the beam such that the tangent along the beam and the cross section axes N1 and N2 form a right-hand rule. This is the data on the second card of the ∗BEAM SECTION option. This is a real vector. This property is required.
Poisson Parameter
Shear Factor
 
Curved Pipe in Space
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Beam in Space
Curved w/Pipe Section
Standard Formulation
Ovalization Only
Ovaliz Only w/ Approx Fourier
Bar/2, Bar/3
Bar/2
Bar/2
Options above create ELBOW31, ELBOW32, ELBOW31B, or C elements depending on the specified options and topology. BEAM SECTION, SECTION=ELBOW properties are also created. ORIENTATION and TRANSVERSE SHEAR STIFFNESS options are created, as required. This defines an elbow element.
More data input is available for creating Curved Pipe in Space elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Property Name
Description
Torus Radius
Defines the radius of the elbow bend. This is one of the data values on the second card of the *BEAM SECTION option. This is either a real constant or a reference to an existing field definition. This property is required.
Integ Points around Pi
Defines the number of integration points to be used around the pipe cross section. This is the second value on the fourth card of the *BEAM SECTION option. This is an integer value. This property is required.
Point Tangents Inters
Defines the orientation of the XY plane of the element coordinate system. This is the data on the second card of the *BEAM SECTION option. This is a Node ID. This property is required.
Integ Points thru Thick
Defines the number of integration points to be used through the pipe wall thickness. This is the first value on the fourth card of the *BEAM SECTION option. This is an integer value.
# Ovalization Modes
Defines the number of ovalization modes to be included in the shape functions of this element. This is the third value of the fourth card of the *BEAM SECTION option. This is an integer value.
Poisson Parameter
Permits an “overall” change of the cross section dimensions as a function of the axial strains. This is the value of the POISSON parameter on the ∗BEAM SECTION option.
Shear Factor
L-Section Beam in Space
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Beam in Space
L-Section
Standard Formulation
Hybrid
Cubic Interpolation
Cubic Hybrid
Cubic Initially Straight
Bar/2, Bar/3
Bar/2, Bar/3
Bar/2
Bar/2
Bar/2
Options above create B31, B32, B33, B34, B31H, B32H, or B33H elements depending on the specified options and topology. BEAM SECTION, SECTION=L properties are also created.
ORIENTATION and TRANSVERSE SHEAR STIFFNESS options are created, as required. This defines an L-section beam.
More data input is available for creating L-Section Beam in Space elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Property Name
Description
Definition of XY Plane
Defines the cross section axis N1 of the beam such that the tangent along the beam and the cross section axes N1 and N2 form a right-hand rule. This is the data on the second card of the *BEAM SECTION option. This is a real vector. This property is required.
Poisson Parameter
Permits an “overall” change of the cross section dimensions as a function of the axial strains. This is the value of the POISSON parameter on the ∗BEAM SECTION option.
Shear Factor
The product of this factor, the beam cross sectional area, and the shear modulus for the material defines the transverse shear stiffness for the beam. This value appears on the ∗TRANSVERSE SHEAR STIFFNESS option.
Open Beam in Space
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Beam in Space
Open Section
Standard Formulation
Hybrid
Bar/2, Bar/3
Bar/2, Bar/3
Options above create B31OS, B32OS, B31OSH, or B32OSH elements depending on the specified options and topology. BEAM GENERAL SECTION, SECTION=GENERAL properties are also created. ORIENTATION and TRANSVERSE SHEAR STIFFNESS options are created, as required. This defines an open section beam.
More data input is available for creating Open Beam in Space elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
 
Property Name
Description
Area Moment I12
Defines the area moment of the element cross section. This is the I12 value on the second card of the *BEAM GENERAL SECTION option. This can be either a real constant or a reference to an existing field definition.
Torsional Constant
Defines the torsional constant of the element cross section. This is the J value on the second card of the *BEAM GENERAL SECTION option. This can be either a real constant or a reference to an existing field definition.
Definition of XY Plane
Defines the cross section axis N1 of the beam such that the tangent along the beam and the cross section axes N1 and N2 form a right-hand rule. This is the data on the second card of the *BEAM GENERAL SECTION option. This is a real vector. This property is required.
1st. Sectorial Moment
This can be either a real constant or a reference to an existing field definition. This property is required for open section beams.
Warping Constant
This can be either a real constant or a reference to an existing field definition. This property is required for open section beams.
Centroid Coord 1
Centroid Coord 2
Defines the location of the centroid of the cross section with respect to the local cross section coordinate system. These values are either real constants or references to existing field definitions. These are the values on the ∗CENTROID suboption of the ∗BEAM GENERAL SECTION option.
Shear Center Coord 1
Shear Center Coord 2
Defines the location of the shear centroid of the cross section with respect to the local cross section coordinate system. These values are either real constants or references to existing field definitions. These are the values on the ∗SHEAR CENTER suboption of the ∗BEAM GENERAL SECTION option.
Poisson Parameter
Shear Factor
Section Point Coord 1
Section Point Coord 2
Defines the coordinates of points in the beam cross section where output is requested. These are lists of real constants. These values are measured in the beam cross section coordinate system. The lists must have the same number of entries. These are the values on the ∗SECTION POINTS suboption of the ∗BEAM GENERAL SECTION option.
Truss
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Truss
Standard Formulation
Hybrid
 
Bar/2. Bar/3
Bar/2. Bar/3
Options above create T3D2, T3D2H, T3D3, or T3D3H elements depending on the specified options and topology. *SOLID SECTION properties are also created. The cross sectional area is included on the *SOLID SECTION option.
Linear Spring (Axial)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Spring
Linear
Standard Formulation
Bar/2
Options above create SPRINGA elements with *SPRING properties. This element defines a linear spring between two nodes whose line of action is the line joining the two nodes.
Linear Spring (Fixed Direction)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Spring
Linear
Fixed Direction
Bar/2
Options above create SPRING2 elements with *SPRING properties.This element defines a linear spring between specified degrees-of-freedoms at two nodes. An *ORIENTATION option may also be created, as required.
 
Nonlinear Spring (Axial)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Spring
Nonlinear
Standard Formulation
Bar/2
Options above create SPRINGA elements with *SPRING properties.This element defines a nonlinear spring between two nodes whose line of action is the line joining the two nodes.
Nonlinear Spring (Fixed Direction)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Spring
Nonlinear
Fixed Direction
Bar/2
Options above create SPRING2 elements with SPRING properties. This element type defines a nonlinear spring between two nodes, acting in a fixed direction. An ORIENTATION option may also be created, as required.
Linear Damper (Axial)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Damper
Linear
Standard Formulation
Bar/2
Options above create DASHPOTA elements with DASHPOT properties. This element type defines a linear damper between two nodes whose line of action is the line joining the two nodes.
Linear Damper (Fixed Direction)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Damper
Linear
Fixed Direction
Bar/2
Options above create DASHPOT2 elements with DASHPOT properties. This element type defines a linear damper between two nodes, acting in a fixed direction. An ORIENTATION option may also be created, as required.
Nonlinear Damper (Axial)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Damper
Nonlinear
Standard Formulation
Bar/2
Options above create DASHPOTA elements with DASHPOT properties. This element type defines a nonlinear damper between two nodes whose line of action is the line joining the two nodes.
Nonlinear Damper (Fixed Direction)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Damper
Nonlinear
Fixed Direction
Bar/2
Options above create DASHPOT2 elements with DASHPOT properties. This element type defines a nonlinear damper between two specified nodes, acting in a fixed direction. An ORIENTATION option may also be created, as required.
Gap (Uniaxial), Gap (Cylindrical)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Gap
Cylindrical
Uniaxial
True Distance
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No Separation
Lagrange Vis Damping
Lagrange Vis Damping No Separation
Bar/2
Options above create GAPUNI or GAPCYL elements with *GAP properties. The ∗FRICTION option is created, as required.
Gap (Spherical)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Gap
Spherical
True Distance
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No Separation
Lagrange Vis Damping
Lagrange Vis Damping No Separation
Bar/2
Options above create GAPSPHER elements with *GAP properties. The *FRICTION option is created, as required.
Axisymmetric Shell
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Axisymmetric Shell
Homogeneous
 
Bar/2 Bar/3
Options above create SAX1 or SAX2 elements, depending on the specified topology, with *SHELL SECTION properties.
Axisymmetric Shell (Laminate)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Axisymmetric Shell
Laminate
 
Bar/2
Options above create SAX1 or SAX2 elements, depending on the specified topology, with SHELL SECTION, COMPOSITE properties.
 
1D Interface
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
1D Interface
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No Separation
Lagrange Vis Damping
Lagrange Vis Damping No Separation
 
Bar/2
Options above create INTER1 elements with *INTERFACE, *FRICTION, and *SURFACE CONTACT properties. The SOFTENED parameter on the *SURFACE CONTACT option may be included, depending on the selected option. This element defines an interface region between two portions of an axisymmetric model. These elements must be created from one contact surface to the other.
More data input is available for creating 1D Interface elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Description
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip tolerance
Defines the value of , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option.
Clearance Zero-Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the ∗SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient
is constant.
Planar ISL (In Plane)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
ISL (in plane)
Planar
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No Separation
Lagrange Vis Damping
Lagrange Vis Damping No Separation
Bar/2, Bar/3
Options above create ISL21 or ISL22 elements (depending on the selected topology) with *INTERFACE and *FRICTION properties. This element defines an interface between the edge of an element on a planar model and another part of the model.
More data input is available for creating Planar ISL (in plane) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Description
Friction in Dir_1
Defines the sliding friction in the element’s 1 direction. This is the friction coefficient on the second card of the *FRICTION option.
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option.
Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Press Zero Clearance
Defines the pressure at zero clearance. This is the value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the *SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative
Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
Axisymmetric ISL (In Plane)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
ISL (in plane)
Axisymmetric
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No Separation
Lagrange Vis Damping
Lagrange Vis Damping No Separation
Bar/2, Bar/3
Options above create ISL21A or ISL22A elements (depending on the selected topology) with *INTERFACE and *FRICTION properties. This element defines an interface between the edge of an element on an axisymmetric model and another part of the model.
More data input is available for creating Axisymmetric ISL (in plane) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Description
Friction in Dir_1
Defines the sliding friction in the element’s 1 direction. This is the friction coefficient on the second card of the *FRICTION option.
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option.
Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Press Zero Clearance
Defines the pressure at zero clearance. This is the value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the *SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the value on the *SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
Parallel ISL (In Space)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
ISL (in space)
Parallel
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No Separation
Lagrange Vis Dampin
Lagrange Vis Damping No Separation
Bar/2, Bar/3
Options above create ISL31 or ISL32 elements (depending on the selected topology) with *INTERFACE and *FRICTION properties. This element type defines an interface between the edge of an element and another part of the model.
More data input is available for creating Parallel ISL (in space) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Description
Friction in Dir_1
Friction in Dir_2
Defines the sliding friction in the element’s 1 and 2 directions. These are the friction coefficients on the second card of the *FRICTION option. If Friction in Dir_2 is specified, then the ANISOTROPIC parameter is included on the *FRICTION option. These values can be either real constants or references to existing field definitions.
Vector
Defines the normal to the plane in which sliding contact occurs. This is the second card of the *INTERFACE option. This value is a global vector. This property is required.
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the *FRICTION option.
Slip Tolerance
Defines the value of , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the *FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the *FRICTION option.
Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the *SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the p0 value on the *SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
Radial ISL (In Space)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
ISL (in space)
Radial
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No Separation
Lagrange Vis Damping
Lagrange Vis Damping No Separation
Bar/2, Bar/3
Options above create ISL31 or ISL32 elements (depending on the selected topology) with *INTERFACE and *FRICTION properties. This element defines an interface between the edge of an element and another part of the model.
More data input is available for creating Radial ISL (in space) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Description
Friction in Dir_1
Friction in Dir_2
Defines the sliding friction in the element’s 1- and 2-directions. These are the friction coefficients on the second card of the ∗FRICTION option. If Friction in Dir_2 is specified, then the ANISOTROPIC parameter is included on the ∗FRICTION option. These values can be either real constants or references to existing field definitions.
Vector
Defines the normal to the plane in which sliding contact occurs. This is the second card of the ∗INTERFACE option. This value is a global vector. This property is required.
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option.
Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the *SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
Slide Line
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Slide Line
 
 
Bar/2, Bar/3
Options above create Slide Lines for the ISL elements. These elements must be equivalenced and continuous.
IRS (Planar)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
IRS (plane/axisym)
Planar
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No Separation
Lagrange Vis Damping
Lagrange Vis Damping No Separation
Bar/2, Bar/3
Options above create IRS21 or IRS22 elements (depending on the selected topology) with *INTERFACE and *FRICTION properties. This element type defines an interface between the edge of a linear element on a planar model and a rigid surface.
More data input is available for creating IRS (planar) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Description
Friction in Dir_1
Defines the sliding friction in the element’s 1 direction. This is the friction coefficient on the second card of the *FRICTION option.
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the *FRICTION option.
Slip Tolerance
Defines the value of , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the *FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the *FRICTION option.
Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points considered not in contact. This is the c value on the *SURFACE CONTACT option.
This property is only used for the Hard Contact option. This is a
real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the value on the *SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
IRS (Axisymmetric)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
IRS (plane/axisym)
Axisymmetric
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No Separation
Lagrange Vis Damping
Lagrange Vis Damping No Separation
Bar/2, Bar/3
Options above create IRS21A or IRS22A elements (depending on the selected topology) with *INTERFACE and *FRICTION properties. This element type defines an interface between the edge of a linear element on an axisymmetric model and a rigid surface.
More data input is available for creating IRS (axisymmetric) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
 
Property Name
Description
Friction in Dir_1
Defines the sliding friction in the element’s 1 direction. This is the friction coefficient on the second card of the *FRICTION option.
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option.
Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points considered not in contact. This is the c value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient
is constant.
IRS (Beam/Pipe)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
IRS (beam/pipe)
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No Separation
Lagrange Vis Damping
Lagrange Vis Damping No Separation
 
Bar/2, Bar/3
Options above create IRS31 or IRS32 elements (depending on the selected topology) with *INTERFACE and *FRICTION properties. This element type defines an interface between a beam or pipe element on a spatial model and a rigid surface.
More data input is available for creating IRS (beam/pipe) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Description
Friction in Dir_1
Friction in Dir_2
Defines the sliding friction in the element’s 1 and 2 directions. These are the friction coefficients on the second card of the *FRICTION option. If Friction in Dir_2 is specified, then the ANISOTROPIC parameter is included on the *FRICTION option. These values can be either real constants or references to existing field definitions.
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the *FRICTION option.
Slip Tolerance
Defines the value of , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the *FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the *FRICTION option.
Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the *SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the value on the *SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Defines the ROUGH parameter on the *FRICTION option. This property is only used for the Lagrange option.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
Rigid Surface (Segments)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Rigid Surf (Seg)
 
 
Bar/2
Options above create a ∗RIGID SURFACE, TYPE=SEGMENTS option (see Section 7.4.7 of the ABAQUS/Standard User’s Manual).
The rigid surface is defined by creating Bar/2 elements. All the elements must be connected and should not have duplicate nodes. The start Point (Node ID) defines the positive progression direction along the surface. The right-handed rotation from this direction defines the outward normal.
Rigid Surface (Cylindrical)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Rigid Surf (Cyl)
 
 
Bar/2
Options above create a ∗RIGID SURFACE, TYPE = CYLINDRICAL option (see Section 7.4.7 of the ABAQUS/Standard User’s Manual).
The rigid surface is first defined by creating Bar/2 elements. All the elements must be connected and should not have duplicate nodes.
The rigid surface’s +x direction is defined from the start point (node ID) along the line of the rigid surface. The +y direction is away from the object the rigid surface will be in contact with. The +z direction (the surface generation vector) is defined by using right-hand rule, crossing the rigid surface’s +x axis with the +y axis.
Rigid Surface (Axisymmetric)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Rigid Surf (Axi)
 
 
Bar/2
Options above create a ∗RIGID SURFACE, TYPE=AXISYMMETRIC option (see Section 7.4.7 of the ABAQUS/Standard User’s Manual).
The rigid surface is defined by creating Bar/2 elements. All the elements must be connected and should not have duplicate nodes. The Start Point defines the positive progression direction along the surface. The right-handed rotation from this direction defines the outward normal.
Rigid Surface (Bezier 2D)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Rigid Surf (Bz2D)
 
 
Bar/2
Options above create a ∗RIGID SURFACE, TYPE=BEZIER option for use in two-dimensional analysis (see Section 7.4.7 of the ABAQUS/Standard User’s Manual).
The rigid surface is defined by creating Bar/2 elements. All the elements must be connected and should not have duplicate nodes. The Start Point defines the positive progression direction along the surface. The right-handed rotation from this direction defines the outward normal.
Rigid Line (LBC)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Rigid Line(LBC)
 
 
Bar/2
This property set is created when the Rigid-Deform contact LBC is created in the Loads/BCs menu. The creation or deletion of this property set is not required by the user. The elements associated with this property set are translated as R2D2 and RAX2 elements.
Rebar
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Rebar
Axisymmetric
General Axisymmetric
 
Bar/2, Bar/3
The options above create SFMAX1, SFMAX2, SFMGAX1 and SFMGAX2 elements (depending on the selected options and topologies) with *SURFACE SECTION properties. The *EMBEDDED ELEMENT and *REBAR LAYER options are also created.
 
Material Name
Defines the material to be used. When entering data here, a list of all isotropic materials in the database is displayed. You can either pick one from the list with the mouse or type in the name. This identifies the material that will be referenced on the *REBAR LAYER option. This property is required.
X-Sectional Area
Defines the area of the rebar cross-section. This is the cross-sectional area value on the *REBAR LAYER option. A real constant, a reference to an existing field definition, or a real list may be entered. A real list is used to specify the cross-sectional area for more than one rebar layer. This property is required.
Spacing
Defines the spacing of the rebars within a layer. This is the spacing value on the *REBAR LAYER option. A real constant, a reference to an existing field definition, or a real list may be entered. A real list is used to specify the spacing for more than one rebar layer. This property is required.
Spacing Unit Type
Defines the unit type for the spacing values. When “Angle” is specified, the ANGULAR SPACING parameter is used for the *REBAR LAYER option. “Distance” is the default value. This property is not required.
Rebar Orient. Angle
Defines the angular orientation of the rebar from the meridional plane in degrees. This is the angular orientation value on the *REBAR LAYER option. A real constant, a reference to an existing field definition, or a real list may be entered. A real list is used to specify the angular orientation for more than one rebar layer. This property is required.
Host Property Set
Defines the element property set of the elements that host the rebar elements. This is the “HOST ELSET” parameter on the *EMBEDDED ELEMENT option. A reference to an existing element property set may be specified. By default, the solver determines the host elements based on the position of the embedded elements within the model. This property is not required.
Roundoff Tolerance
Defines the value below which the weigh factors of the host element’s nodes will be zeroed out. This is the ROUNDOFF TOLERANCE parameter on the *EMBEDDED ELEMENT option. A real scalar may be specified. The default value is 1E+6. This property is not required.
Mech Joint (2D Model) - ALIGN
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (2D Model)
ALIGN
 
Bar/2
This option creates CONN2D2 elements. The connection type is set to ALIGN on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Mech Joint (2D Model) - AXIAL
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (2D Model)
AXIAL
 
Bar/2
This option creates CONN2D2 elements. The connection type is set to AXIAL on the *CONNECTOR SECTION option.
 
 
Force/Disp, X Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. Use a real constant or a non-spatial field to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Zero Force Ref Len
This property value defines the reference length of the unloaded connector element. This value is translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real constant to specify this property.
Damping, X Axis
This damping property value defines the relationship between force and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or a non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is force, and velocity is a required independent variable.
Connector Min Stop
This property value defines a lower limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Connector Max Stop
This property value defines an upper limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Friction Lim, X Axis
This property value defines the force limit associated with the friction portion of the connector element. This value is translated to the ABAQUS input file with the *CONNECTOR FRICTION option. A real constant or a non-spatial field may be used to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define a limit that varies with temperature and/or displacement. The dependent variable for these fields is force.
Friction Stick Stiff
This property value defines the stiffness associated with the friction portion of the connector element. This value appears as the STICK STIFFNESS parameter in the *CONNECTOR FRICTION option. Use a real constant to specify this property.
Lock, Min Disp
This property value defines the lower bound on the relative position that triggers a locked condition in the connector element. This value is translated to the ABAQUS input file with the *CONNECTOR LOCK option. Use a real constant to specify this property.
Mech Joint (2D Model) - BEAM
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (2D Model)
BEAM
 
Bar/2
This option creates CONN2D2 elements. The connection type is set to BEAM on the *CONNECTOR SECTION option.
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Mech Joint (2D Model) - CARTESIAN
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (2D Model)
CARTESIAN
 
Bar/2
This option creates CONN2D2 elements. The connection type is set to CARTESIAN on the *CONNECTOR SECTION option.
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Force/Disp, X Axis
Force/Disp, Y Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. Use a real constant or a non-spatial field to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Zero Force Ref Len
These property values define the reference lengths for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Damping, X Axis
Damping, Y Axis
This damping property value defines the relationship between force and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or a non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is force, and velocity is a required independent variable.
Connector Min Stop
These property values define the lower limits for the components of the connector's relative position. These values are translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real vector to specify this property.
Connector Max Stop
These property values define the upper limits for the components of the connector's relative position. These values are translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real vector to specify this property.
Mech Joint (2D Model) - JOIN
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (2D Model)
JOIN
 
Bar/2
This option creates CONN2D2 elements. The connection type is set to JOIN on the *CONNECTOR SECTION option.
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Mech Joint (2D Model) - JOINTC
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (2D Model)
JOINTC
 
Bar/2
This option creates JOINTC elements. The *JOINT, *SPRING and *DASHPOT options are used to define the properties.
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *JOINT option. Use an existing coordinate system to specify this property.
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
Force/Disp, X Axis
Force/Disp, Y Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *SPRING option. A real constant or a non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Mom/Rot about Z Axis
This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *SPRING option. A real constant or a non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Damping, X Axis
Damping, Y Axis
This damping property value defines the relationship between force and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *DASHPOT option. A real constant or non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be
used to define damping that varies with velocity and temperature. The dependent variable for these fields is force, and velocity is a required independent variable.
Rot Damping, Z Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *DASHPOT option. A real constant or a non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be
used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Mech Joint (2D Model) - LINK
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (2D Model)
LINK
 
Bar/2
This option creates CONN2D2 elements. The connection type is set to LINK on the *CONNECTOR SECTION option.
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Mech Joint (2D Model) - ROTATION
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (2D Model)
ROTATION
 
Bar/2
This option creates CONN2D2 elements. The connection type is set to ROTATION on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
Mom/Rot about Z Axis
This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. A real constant or a non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Zero Moment Ref Ang
This property value defines the reference angle of the unloaded connector element. This value is translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real constant to specify this property.
Rot Damping, Z Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Connector Min Stop
This property value defines a lower limit for the connector's relative position. This value is translated to the ABAQUS input file with
the *CONNECTOR STOP option. Use a real constant to specify
this property.
Connector Max Stop
This property value defines an upper limit for the connector's relative position. This value is translated to the ABAQUS input file with
the *CONNECTOR STOP option. Use a real constant to specify
this property.
 
Mech Joint (2D Model) - SLOT
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (2D Model)
SLOT
 
Bar/2
This option creates CONN2D2 elements. The connection type is set to SLOT on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Force/Disp, X Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. Use a real constant or a non-spatial field to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Zero Force Ref Len
This property value defines the reference length of the unloaded connector element. This value is translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real constant to specify this property.
Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Connector Min Stop
This property value defines a lower limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Connector Max Stop
This property value defines an upper limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Friction Lim, X Axis
This property value defines the force limit associated with the friction portion of the connector element. This value is translated to the ABAQUS input file with the *CONNECTOR FRICTION option. A real constant or a non-spatial field may be used to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define a limit that varies with temperature and/or displacement. The dependent variable for these fields is force.
Friction Stick Stiff
This property value defines the stiffness associated with the friction portion of the connector element. This value appears as the STICK STIFFNESS parameter in the *CONNECTOR FRICTION option. Use a real constant to specify this property.
Mech Joint (2D Model) - TRANSLATOR
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (2D Model)
TRANSLATOR
 
Bar/2
This option creates CONN2D2 elements. The connection type is set to TRANSLATOR on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Mech Joint (2D Model) - WELD
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (2D Model)
WELD
 
Bar/2
This option creates CONN2D2 elements. The connection type is set to WELD on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Mech Joint (3D Model) - ALIGN
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (3D Model)
ALIGN
 
Bar/2
This option creates CONN3D2 elements. The connection type is set to ALIGN on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Mech Joint (3D Model) - AXIAL
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (3D Model)
AXIAL
 
Bar/2
This option creates CONN3D2 elements. The connection type is set to AXIAL on the *CONNECTOR SECTION option.
 
Force/Disp, X Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. Use a real constant or a non-spatial field to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Zero Force Ref Len
This property value defines the reference length of the unloaded connector element. This value is translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real constant to specify this property.
Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Connector Min Stop
This property value defines a lower limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Connector Max Stop
This property value defines an upper limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Friction Lim, X Axis
This property value defines the force limit associated with the friction portion of the connector element. This value is translated to the ABAQUS input file with the *CONNECTOR FRICTION option. A real constant or a non-spatial field may be used to specify this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define a limit that varies with temperature and/or displacement. The dependent variable for these fields is force.
Friction Stick Stiff
This property value defines the stiffness associated with the friction portion of the connector element. This value appears as the STICK STIFFNESS parameter in the *CONNECTOR FRICTION option. Use a real constant to specify this property.
Lock Min Disp
This property value defines the upper bound on the relative position that triggers a locked condition in the connector element. This value is translated to the ABAQUS input file with the *CONNECTOR LOCK option. Use a real constant to specify this property.
Mech Joint (3D Model) - BEAM
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (3D Model)
BEAM
 
Bar/2
This option creates CONN3D2 elements. The connection type is set to BEAM on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Mech Joint (3D Model) - CARDAN
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (3D Model)
CARDAN
 
Bar/2
This option creates CONN3D2 elements. The connection type is set to CARDAN on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
Mom/Rot about X Axis
Mom/Rot about Y Axis
Mom/Rot about Z Axis
This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. A real constant or a non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Zero Moment Ref Ang
These property values define the reference angles for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Rot Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Mech Joint (3D Model) - CARTESIAN
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (3D Model)
CARTESIAN
 
Bar/2
This option creates CONN3D2 elements. The connection type is set to CARTESIAN on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Force/Disp, X Axis
Force/Disp, YAxis
Force/Disp, Z Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. Use a real constant or a non-spatial field to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Zero Force Ref Len
These property values define the reference angles for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Damping, X Axis
Damping, Y Axis
Damping, Z Axis
This damping property value defines the relationship between force and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or a non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is force, and velocity is a required independent variable.
Mech Joint (3D Model) - CONSTANT VELOCITY
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (3D Model)
CONSTANT VELOCITY
 
Bar/2
This option creates CONN3D2 elements. The connection type is set to CONSTANT VELOCITY on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify
this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file
with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify
this property.
Mech Joint (3D Model) - CVJOINT
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (3D Model)
CVJOINT
 
Bar/2
This option creates CONN3D2 elements. The connection type is set to CVJOINT on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Mech Joint (3D Model) - CYLINDRICAL
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (3D Model)
CYLINDRICAL
 
Bar/2
This option creates CONN3D2 elements. The connection type is set to CYLINDRICAL on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify
this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify
this property.
Mech Joint (3D Model) - EULER
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (3D Model)
EULER
 
Bar/2
This option creates CONN3D2 elements. The connection type is set to EULER on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
Mom/Rot about X Axis
Mom/Rot about Y Axis
Mom/Rot about Z Axis
This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. A real constant or a non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Zero Moment Ref Ang
These property values define the reference angles for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Rot Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Mech Joint (3D Model) - FLEXION-TORSION
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (3D Model)
FLEXION-TORSION
 
Bar/2
This option creates CONN3D2 elements. The connection type is set to FLEXION-TORSION on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
Mom/Rot about X Axis
Mom/Rot about Y Axis
Mom/Rot about Z Axis
This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. A real constant or a non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Zero Moment Ref Ang
These property values define the reference angles for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Rot Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Mech Joint (3D Model) - HINGE
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (3D Model)
HINGE
 
Bar/2
This option creates CONN3D2 elements. The connection type is set to HINGE on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Mech Joint (3D Model) - JOIN
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (3D Model)
JOIN
 
Bar/2
This option creates CONN3D2 elements. The connection type is set to JOIN on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Mech Joint (3D Model) - JOINTC
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (3D Model)
JOINTC
 
Bar/2
This option creates JOINTC elements. The *JOINT, *SPRING and *DASHPOT options are used to define the properties.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *JOINT option. Use an existing coordinate system to specify this property.
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
Force/Disp, X Axis
Force/Disp, Y Axis
Force/Disp, Z Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *SPRING option. A real constant or a non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required
independent variable.
Mom/Rot about X Axis
Mom/Rot about Y Axis
Mom/Rot about Z Axis
This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *SPRING option. A real constant or a non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Mech Joint (3D Model) - LINK
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (3D Model)
LINK
 
Bar/2
This option creates CONN3D2 elements. The connection type is set to LINK on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Mech Joint (3D Model) - PLANAR
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (3D Model)
PLANAR
 
Bar/2
This option creates CONN3D2 elements. The connection type is set to PLANAR on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Mech Joint (3D Model) - RADIAL-THRUST
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (3D Model)
RADIAL-THRUST
 
Bar/2
This option creates CONN3D2 elements. The connection type is set to RADIAL-THRUST on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Force/Disp, X Axis
Force/Disp, ZAxis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. Use a real constant or a non-spatial field to specify this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Zero Force Ref Len
These property values define the reference lengths for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Damping, X Axis
Damping, Z Axis
This damping property value defines the relationship between force and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or a non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is force, and velocity is a required independent variable.
Connector Min Stop
These property values define the lower limits for the components of the connector's relative position. These values are translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real vector to specify this property.
Connector Max Stop
These property values define the upper limits for the components of the connector's relative position. These values are translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real vector to specify this property.
Mech Joint (3D Model) - REVOLUTE
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (3D Model)
REVOLUTE
 
Bar/2
This option creates CONN3D2 elements. The connection type is set to REVOLUTE on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
Mom/Rot about X Axis
This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. A real constant or a non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Zero Moment Ref Ang
This property value defines the reference angle of the unloaded connector element. This value is translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real constant to specify this property.
Rot Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Connector Min Stop
This property value defines a lower limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Connector Max Stop
This property value defines an upper limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Mech Joint (3D Model) - ROTATION
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (3D Model)
ROTATION
 
Bar/2
This option creates CONN3D2 elements. The connection type is set to ROTATION on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
Mom/Rot about X Axis
Mom/Rot about Y Axis
Mom/Rot about Z Axis
This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. A real constant or a non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Zero Moment Ref Ang
These property values define the reference angles for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Rot Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Mech Joint (3D Model) - SLIDE-PLANE
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (3D Model)
SLIDE-PLANE
 
Bar/2
This option creates CONN3D2 elements. The connection type is set to SLIDE-PLANE on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify
this property.
Force/Disp, Y Axis
Force/Disp, Z Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. Use a real constant or a non-spatial field to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Zero Force Ref Len
These property values define the reference lengths for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Damping, Y Axis
Damping, Z Axis
This damping property value defines the relationship between force and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or a non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is force, and velocity is a required independent variable.
Connector Min Stop
These property values define the lower limits for the components of the connector's relative position. These values are translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real vector to specify this property.
Connector Max Stop
These property values define the upper limits for the components of the connector's relative position. These values are translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real vector to specify this property.
Mech Joint (3D Model) - SLOT
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (3D Model)
SLOT
 
Bar/2
This option creates CONN3D2 elements. The connection type is set to SLOT on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Force/Disp, X Axis
This stiffness property value defines the relationship between force and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. Use a real constant or a non-spatial field to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is force, and displacement is a required independent variable.
Zero Force Ref Len
This property value defines the reference length of the unloaded connector element. This value is translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real constant to specify this property.
Damping, X Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Connector Min Stop
This property value defines a lower limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Connector Max Stop
This property value defines an upper limit for the connector's relative position. This value is translated to the ABAQUS input file with the *CONNECTOR STOP option. Use a real constant to specify this property.
Friction Lim, X Axis
This property value defines the force limit associated with the friction portion of the connector element. This value is translated to the ABAQUS input file with the *CONNECTOR FRICTION option. A real constant or a non-spatial field may be used to specify this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define a limit that varies with temperature and/or displacement. The dependent variable for these fields is force.
Friction Stick Stiff
This property value defines the stiffness associated with the friction portion of the connector element. This value appears as the STICK STIFFNESS parameter in the *CONNECTOR FRICTION option. Use a real constant to specify this property.
Mech Joint (3D Model) - TRANSLATOR
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (3D Model)
TRANSLATOR
 
Bar/2
This option creates CONN3D2 elements. The connection type is set to TRANSLATOR on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Mech Joint (3D Model) - UJOINT
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (3D Model)
UJOINT
 
Bar/2
This option creates CONN3D2 elements. The connection type is set to UJOINT on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Mech Joint (3D Model) - UNIVERSAL
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (3D Model)
UNIVERSAL
 
Bar/2
This option creates CONN3D2 elements. The connection type is set to UNIVERSAL on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Units for Angles
This property determines the units for the angle values. It may be set to either "Degrees" or "Radians". The default value is "Radians".
Mom/Rot about X Axis
Mom/Rot about Z Axis
This stiffness property value defines the relationship between moment and relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR ELASTICITY option. A real constant or a non-spatial field may be used for this property. The n on-spatial fields that have been created with the “Tabular Input” method may be used to define stiffness that varies with displacement and temperature. The dependent variable for this field is moment, and displacement is a required independent variable.
Zero Moment Ref Ang
These property values define the reference angles for the components of the unloaded connector element. These values are translated to the ABAQUS input file with the *CONNECTOR CONSTITUTIVE REFERENCE option. Use a real vector to specify this property.
Rot Damping, X Axis
Rot Damping, Z Axis
This damping property value defines the relationship between moment and the rate of change of relative displacement in the connector element. It is translated to the ABAQUS input file with the *CONNECTOR DAMPING option. A real constant or non-spatial field may be used for this property. The non-spatial fields that have been created with the “Tabular Input” method may be used to define damping that varies with velocity and temperature. The dependent variable for these fields is moment, and velocity is a required independent variable.
Mech Joint (3D Model) - WELD
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
Mech Joint (3D Model)
WELD
 
Bar/2
This option creates CONN3D2 elements. The connection type is set to WELD on the *CONNECTOR SECTION option.
 
Node A Analysis CID
This property defines the directions for the degrees of freedom at the first node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Node B Analysis CID
This property defines the directions for the degrees of freedom at the second node of the connector element. It is translated to the ABAQUS input file with an *ORIENTATION option and is referenced from the *CONNECTOR SECTION option. Use an existing coordinate system to specify this property.
Axisym Link Gasket
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
1D Gasket
Axisymmetric Link
Gasket Behavior Model
Bar2
These options create GKAX2 elements. The *GASKET SECTION option is used to define the gasket thickness, width, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the membrane and transverse shear behaviors.
 
Membrane Material
This property defines the membrane material to be used. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to MEMBRANE. The Elastic Modulus and Poisson's Ratio may vary with temperature. This property is not required.
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
F/L vs. Closure (Loading)
This property defines the force per unit length versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
F/L vs. Closure (Unloading)
This property defines the force per unit length versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Shear Stiffness
This property defines the shear stiffness of the gasket elements. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to TRANSVERSE SHEAR. A real constant or a non-spatial field may be used to define this property. The non-spatial fields that have been created with the "Tabular Input" method may be used to define shear stiffness that varies with temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Width
This property defines the width of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Axisym Link Gasket (Thick only)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
1D Gasket
Axisymmetric Link
Thickness Behavior Only
Bar2
These options create GKAX2N elements. The *GASKET SECTION option is used to define the gasket thickness, width, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction.
 
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
F/L vs. Closure (Loading)
This property defines the force per unit length versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
F/L vs. Closure (Unloading)
This property defines the force per unit length versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Width
This property defines the width of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Axisym Link Gasket (Material)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
1D Gasket
Axisymmetric Link
Built-in Material
Bar2
These options create GKAX2 elements. The *GASKET SECTION option is used to define the gasket thickness, width, initial gap and initial void values. The gasket material is specified using the MATERIAL parameter on the *GASKET SECTION option.
 
Material Name
This property defines the material to be used. It is translated to the ABAQUS input file as the MATERIAL parameter on the *GASKET SECTION option. This property is required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Width
This property defines the width of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
3D Link Gasket
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
1D Gasket
3D Link
Gasket Behavior Model
Bar2
These options create GK3D2 elements. The *GASKET SECTION option is used to define the gasket thickness, x-sectional area, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the transverse shear behavior.
 
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
F vs. Closure (Loading)
This property defines the force versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
F vs. Closure (Unloading)
This property defines the force versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Shear Stiffness
This property defines the shear stiffness of the gasket elements. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to TRANSVERSE SHEAR. A real constant or a non-spatial field may be used to define this property. The non-spatial fields that have been created with the "Tabular Input" method may be used to define shear stiffness that varies with temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
X-Sectional Area
This property defines the x-sectional area of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Orientation System
This property defines the coordinate system to use in defining the local two and three directions for the gasket elements. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. An existing coordinate frame may be used to define this property. This property is not required.
Orientation Axis
This property defines the axis of rotation of the Orientation System for the Orientation Angle. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. An integer value of 1, 2 or 3 may be used to define this property. This property is not required. The default value is 1.
Orientation Angle
This property defines the additional rotation about the Orientation Axis in degrees. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
3D Link Gasket (Thick only)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
1D Gasket
3D Link
Thickness Behavior Only
Bar2
These options create GK3D2N elements. The *GASKET SECTION option is used to define the gasket thickness, x-sectional area, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction.
 
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
F vs. Closure (Loading)
This property defines the force versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
F vs. Closure (Unloading)
This property defines the force versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
X-Sectional Area
This property defines the x-sectional area of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
3D Link Gasket (Material)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
1D Gasket
3D Link
Built-in Material
Bar2
These options create GK3D2 elements. The *GASKET SECTION option is used to define the gasket thickness, x-sectional area, initial gap and initial void values. The gasket material is specified using the MATERIAL parameter on the *GASKET SECTION option.
 
Material Name
This property defines the material to be used. It is translated to the ABAQUS input file as the MATERIAL parameter on the *GASKET SECTION option. This property is required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
X-Sectional Area
This property defines the x-sectional area of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Orientation System
This property defines the coordinate system to use in defining the local two and three directions for the gasket elements. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. An existing coordinate frame may be used to define this property. This property is
not required.
Orientation Axis
This property defines the axis of rotation of the Orientation System for the Orientation Angle. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. An integer value of 1, 2 or 3 may be used to define this property. This property is not required. The default value is 1.
Orientation Angle
This property defines the additional rotation about the Orientation Axis in degrees. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
2D Link Gasket
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
1D Gasket
2D Link
Gasket Behavior Model
Bar2
These options create GK2D2 elements. The *GASKET SECTION option is used to define the gasket thickness, x-sectional area, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the transverse shear behavior.
 
 
 
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
F vs Closure (Loading)
This property defines the force versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
F vs Closure (Unloading)
This property defines the force versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Shear Stiffness
This property defines the shear stiffness of the gasket elements. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to TRANSVERSE SHEAR. A real constant or a non-spatial field may be used to define this property. The non-spatial fields that have been created with the "Tabular Input" method may be used to define shear stiffness that varies with temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
X-Sectional Area
This property defines the x-sectional area of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
2D Link Gasket (Thick only)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
1D Gasket
2D Link
Thickness Behavior Only
Bar2
These options create GK2D2N elements. The *GASKET SECTION option is used to define the gasket thickness, x-sectional area, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction.
 
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
F vs Closure (Loading)
This property defines the force versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
F vs Closure (Unloading)
This property defines the force versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
X-Sectional Area
This property defines the x-sectional area of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
2D Link Gasket (Material)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
1D
1D Gasket
2D Link
Built-in Material
Bar2
These options create GK2D2 elements. The *GASKET SECTION option is used to define the gasket thickness, x-sectional area, initial gap and initial void values. The gasket material is specified using the MATERIAL parameter on the *GASKET SECTION option.
 
Material Name
This property defines the material to be used. It is translated to the ABAQUS input file as the MATERIAL parameter on the *GASKET SECTION option. This property is required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
X-Sectional Area
This property defines the x-sectional area of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Thin Shell
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
Shell
Thin Shell
Homogeneous
Tri/3, Quad/4, Tri/6, Quad/8, Quad/9
Options above create STRI35, STRI65, S4R5, S8R5, or S9R5 elements with *SHELL SECTION properties. *ORIENTATION, *TRANSVERSE SHEAR STIFFNESS, and *HOURGLASS STIFFNESS options may also be created, as required. This element defines a standard thin shell element.
More data input is available for creating Thin Shell elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Property Name
Description
Orientation System
Defines the orientation of the material within the shell element. This is a reference to an existing coordinate system. The referenced coordinate system defines the data used to create the *ORIENTATION option.
Ave Shear Stiffness
Defines the transverse shear stiffness. This is the value on the *TRANSVERSE SHEAR STIFFNESS option. This is either a real constant or a reference to an existing field definition.
Membrane Hourglass Stiffness
Normal Hourglass Stiffness
Bending Hourglass Stiffness
Define the artificial stiffness for hourglass control in membrane, normal, and bending modes. These define parameters on the *HOURGLASS STIFFNESS option. These can be either real constants or references to existing field definitions.
Thin Shell (Laminated)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
Shell
Thin Shell
Laminate
Tri/3, Quad/4, Tri/6, Quad/8, Quad/9
Options above create STRI35, STRI65, S4R5, S8R5, or S9R5 elements with *SHELL SECTION properties. *ORIENTATION and ∗TRANSVERSE SHEAR STIFFNESS options may also be created, as required. This defines a laminate thin shell element.
Thick Shell
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
Shell
Thick Shell
Homogeneous
Tri/3, Quad/4, Tri/6, Quad/8
Options above create S3R, STRI65, S4R, or S8R elements with *SHELL SECTION properties. *ORIENTATION, *TRANSVERSE SHEAR STIFFNESS and *HOURGLASS STIFFNESS options may also be created, as required. This defines a homogeneous thick shell element.
More data input is available for creating Thick Shell elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
Property Name
Description
Orientation System
Defines the orientation of the material within the shell element. This is a reference to an existing coordinate system. The referenced coordinate system defines the data used to create the *ORIENTATION option.
Shear Stiffness K13
Shear Stiffness K23
Defines the transverse shear stIffness. These are the values on the *TRANSVERSE SHEAR STIFFNESS option. These are either real constants or references to existing field definitions.
Membrane Hourglass Stiffness
Normal Hourglass Stiffness
Bending Hourglass Stiffness
Define the artificial stIffness for hourglass control in membrane, normal, and bending modes. These define parameters on the *HOURGLASS STIFFNESS option. These can be either real constants or references to existing field definitions.
Thick Shell (Laminated)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
Shell
Thick Shell
Laminate
Tri/3, Quad/4, Tri/6, Quad/8
Options above create S3R, STRI65, S4R, or S8R elements with *SHELL SECTION properties. *ORIENTATION and ∗TRANSVERSE SHEAR STIFFNESS options may also be created, as required. This defines a laminate thick shell element.
General Thin
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
Shell
General Thin Shell
Homogenous
Tri/3, Quad/4, Tri/6, Quad/8, Quad/9
Options above create STRI35, STRI65, S4R5, S8R5, or S9R5 elements with *SHELL GENERAL SECTION properties. *ORIENTATION, *TRANSVERSE SHEAR STIFFNESS, and *HOURGLASS STIFFNESS options may also be created, as required. This defines a general thin shell element.
More data input is available for creating General Thin Shell elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
 
Property Name
Description
Section Stiffness D14
Section Stiffness D24
Section Stiffness D34
Section Stiffness D44
Section Stiffness D15
Section Stiffness D25
Section Stiffness D35
Section Stiffness D45
Section Stiffness D55
Section Stiffness D16
Section Stiffness D26
Section Stiffness D36
Section Stiffness D46
Section Stiffness D56
Section Stiffness D66
Defines the symmetric half of the [D] section stiffness matrix on the *SHELL GENERAL SECTION option. These properties are required.
Force Vector {F1..F6}
Defines the 6 values of the {F} vector on the *SHELL GENERAL SECTION option. This vector defines the generalized stresses caused by a fully constrained unit temperature rise. This is a list of 6 real constants. This property is required.
Temperature Scaling
Thermal Expansion Scaling
Temperature Values
Define the temperature effects on the *SHELL GENERAL SECTION option. These are lists of real values. Each list must have the same number of values. These values are optional.
Orientation System
Defines the orientation of the material within the shell element. This is a reference to an existing coordinate system. The referenced coordinate system defines the data used to create the *ORIENTATION option.
Reference Temperature
Defines the reference temperature for all thermal effects on this element. This defines the ZERO parameter on the *SHELL GENERAL SECTION option.
Density, mass/area
Defines the mass per unit area for the shell element. This is the DENSITY parameter on the *SHELL GENERAL SECTION option. This value can be either a real constant or a reference to an existing field definition.
Ave Shear Stiffness
Defines the transverse shear stiffness. This is the value on the *TRANSVERSE SHEAR STIFFNESS option. This is either a real constant or a reference to an existing field definition.
Membrane Hourglass Stiffness
Normal Hourglass Stiffness
Bending Hourglass Stiffness
Define the artificial stiffness for hourglass control in membrane, normal, and bending modes. These define parameters on the *HOURGLASS STIFFNESS option. These can be either real constants or references to existing field definitions.
 
General Thin Shell (Laminated)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
Shell
General Thin Shell
Laminate
Tri/3, Quad/4, Tri/6, Quad/8, Quad/9
Options above create STRI3, STRI65, S4R5, S8R5 or S9R5 elements with *SHELL GENERAL SECTION properties. *ORIENTATION and ∗TRANSVERSE SHEAR STIFFNESS options may also be created, as required. This defines a laminate thin shell element.
 
General Thick
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
Shell
General Thick Shell
 
Tri/3, Quad/4, Tri/6, Quad/8
Options above create S3R, STRI65, S4R, or S8R elements with *SHELL GENERAL SECTION properties. *ORIENTATION, *TRANSVERSE SHEAR STIFFNESS, and *HOURGLASS STIFFNESS options may also be created, as required. This defines a general thick shell element.
More data input is available for creating General Thick Shell elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
 
Property Name
Description
Section Stiffness D14
Section Stiffness D24
Section Stiffness D34
Section Stiffness D44
Section Stiffness D15
Section Stiffness D25
Section Stiffness D35
Section Stiffness D45
Section Stiffness D55
Section Stiffness D16
Section Stiffness D26
Section Stiffness D36
Section Stiffness D46
Section Stiffness D56
Section Stiffness D66
Defines the symmetric half of the [D] section stiffness matrix on the *SHELL GENERAL SECTION option. These properties are required.
Force Vector {F1..F6}
Defines the 6 values of the {F} vector on the *SHELL GENERAL SECTION option. This vector defines the generalized stresses caused by a fully constrained unit temperature rise. This is a list of 6 real constants. This property is required.
Temperature Scaling
Thermal Expansion Scaling
Temperature Values
Define the temperature effects on the *SHELL GENERAL SECTION option. These are lists of real values. Each list must have the same number of values. These values are optional.
Orientation System
Defines the orientation of the material within the shell element. This is a reference to an existing coordinate system. The referenced coordinate system defines the data used to create the *ORIENTATION option.
Reference Temperature
Defines the reference temperature for all thermal effects on this element. This defines the ZERO parameter on the *SHELL GENERAL SECTION option.
Density, mass/area
Defines the mass per unit area for the shell element. This is the DENSITY parameter on the *SHELL GENERAL SECTION option. This value can be either a real constant or a reference to an existing field definition.
Shear Stiffness K13
Shear Stiffness K23
Defines the transverse shear stiffness. These are the values on the *TRANSVERSE SHEAR STIFFNESS option. These are either real constants or references to existing field definitions.
Membrane Hourglass Stiffness
Normal Hourglass Stiffness
Bending Hourglass Stiffness
Define the artificial stiffness for hourglass control in membrane, normal, and bending modes. These define parameters on the *HOURGLASS STIFFNESS option. These can be either real constants or references to existing field definitions.
 
General Thick Shell (Laminated)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
Shell
General Thick Shell
Laminate
Tri/3, Quad/4, Tri/6, Quad/8, Quad/9
Options above create S3R, STRI65, S4R, or S8R elements with *SHELL GENERAL SECTION properties. *ORIENTATION and ∗TRANSVERSE SHEAR STIFFNESS options may also be created, as required. This defines a laminate thick shell element.
Large Strain
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
Shell
Large Strain Shell
 
Tri/3, Quad/4, Tri/6, Quad/8
Options above create S3R, S4R, or S8R elements with ∗SHELL SECTION properties. ∗ORIENTATION, ∗TRANSVERSE SHEAR STIFFNESS, and ∗HOURGLASS STIFFNESS options may also be created, as required. This defines a large strain element.
More data input is available for creating Large Strain Shell elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu
.
Property Name
Description
Membrane Hourglass Stiff
Normal Hourglass Stiff
Bending Hourglass Stiff
Define the artificial stiffness for hourglass control in membrane, normal, and bending modes. These define parameters on the ∗HOURGLASS STIFFNESS option.
These can be either real constants or references to existing field definitions.
General Large Strain
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
Shell
General Large Strain Shell
 
Tri/3, Quad/4
Options above create S3R, S4R, or S8R elements with ∗SHELL GENERAL SECTION properties. ∗ORIENTATION, ∗TRANSVERSE SHEAR STIFFNESS, and ∗HOURGLASS STIFFNESS options may also be created, as required. This defines a general large strain element.
More data input is available for creating General Large Strain Shell elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu.
 
Property Name
Description
Section Stiffness D14
Section Stiffness D24
Section Stiffness D34
Section Stiffness D44
Section Stiffness D15
Section Stiffness D25
Section Stiffness D35
Section Stiffness D45
Section Stiffness D55
Section Stiffness D16
Section Stiffness D26
Section Stiffness D36
Section Stiffness D46
Section Stiffness D56
Section Stiffness D66
Defines the symmetric half of the [D] section stiffness matrix on the ∗SHELL GENERAL SECTION option.
These properties are required.
Force Vector F1...F6
Defines the 6 values of the {F} vector on the ∗SHELL GENERAL SECTION option. This vector defines the generalized stresses caused by a fully constrained unit temperature rise. This is a list of 6 real constants. This property is required.
Temperature Scaling D
Thermal Expansion Scaling
Temperature Values
Define the temperature effects on the ∗SHELL GENERAL SECTION option. These are lists of real values. Each list must have the same number of values. These values are optional.
Orientation System
Defines the orientation of the material within the shell element. This is a reference to an existing coordinate system. The referenced coordinate system defines the data used to create the ∗ORIENTATION option.
Reference Temperature
Defines the reference temperature for all thermal effects on this element. This defines the ZERO parameter on the ∗SHELL GENERAL SECTION option.
Density, mass/area
Defines the mass per unit surface area for the shell element. This is the DENSITY parameter on the ∗SHELL GENERAL SECTION option. This value can be either a real constant or a reference to an existing field definition.
Poisson Parameter
Permits an “overall” change of the cross section dimensions as a function of the axial strains. This is the value of the POISSON parameter on the *SHELL GENERAL SECTION option.
Shear Stiffness K13
Shear Stiffness K23
Defines the transverse shear stiffness. These are the values on the ∗TRANSVERSE SHEAR STIFFNESS option. These are either real constants or references to existing field definitions.
Membrane Hourglass Stiffness
Normal Hourglass Stiffness
Bending Hourglass Stiffness
Define the artificial stiffness for hourglass control in membrane, normal, and bending modes. These define parameters on the ∗HOURGLASS STIFFNESS option. These can be either real constants or references to existing field definitions.
Plane Strain
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
2D Solid
Plane Strain
Standard Formulation
Hybrid
Hybrid/Reduced Integration
Reduced Integration
Incompatible Modes
Hybrid/Incompatible Modes
Modified Formulation
Modified/Hybrid
Tri/3, Quad/4, Tri/6, Quad/8
 
 
 
 
Tri/6
Tri/6
Options above create CPE3, CPE4, CPE4R, CPE6, CPE6M, CPE8, CPE8R, CPE3H, CPE4H, CPE4RH, CPE6H, CPE6MH, CPE8H, or CPE8RH (depending on the selected options and topologies) elements with *SOLID SECTION properties. The thickness value on the *SOLID SECTION option is included. *ORIENTATION and *HOURGLASS STIFFNESS options may also be included, as required. If triangular element are found where reduced integration is requested, standard integration elements will be used
.
Generalized Plane Strain
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
2D Solid
General Plane
Strain
Standard Formulation
Hybrid
Hybrid/Reduced Integration
Reduced Integration
Incompatible Modes
Hybrid/Incompatible Modes
Tri/3, Quad/4
Tri/6, Quad/8
These options create CGPE5, CGPE5H, CGPE6, CGPE6H, CGPE6I, CGPE6IH, CGPE6R, CGPE6RH, CGPE8, CGPE8H, CGPE10, CGPE10H, CGPE10R or CGPE10RH elements with *SOLID SECTION properties when writing an ABAQUS V5.X or V4.X input file. Otherwise, they create CPEG3, CPEG3H, CPEG4, CPEG4H, CPEG4I, CPEG4IH, CPEG4R, CPEG4RH, CPEG6, CPEG6H, CPEG8, CPEG8H, CPEG8R or CPEG8RH elements with *SOLID SECTION properties. The thickness value on the *SOLID SECTION option is included. *ORIENTATION and *HOURGLASS STIFFNESS options may also be included, as required. If triangular elements are found where reduced integration is requested, standard integration elements will be used.
 
Property Name
Description
[Reference Node] V6.X+
Defines the REF NODE parameter on the *SOLID SECTION option. The third degree of freedom of this node defines the change in length between the bounding planes. The fourth and fifth degrees of freedom of this node define the relative rotations of one bounding plane with respect to the other. This property is required when generating an ABAQUS version 6 or greater input file.
[Node A: DOF<UZ>] V5.X
This property is required when generating an ABAQUS version 4 or 5 input file.
[Node B: DOF<RX,RY] V5.X
This property is required when generating an ABAQUS version 4 or 5 input file.
Plane Stress
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
2D Solid
Plane Stress
Standard Formulation
Reduced Integration
Incompatible Modes
Modified Formulation
Tri/3, Quad/4, Tri/6, Quad/8
 
Tri/6
Options above create CPS3, CPS4, CPS4R, CPS6, CPS6M, CPS8, or CPS8R (depending on the selected options and topologies) elements with *SOLID SECTION properties. The thickness value on the *SOLID SECTION option will be included. *ORIENTATION and *HOURGLASS STIFFNESS options may also be created, as required. If triangular elements are found where reduced integration is requested, standard integration elements will be used.
Axisymmetric Solid
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
2D Solid
Axisymmetric
Standard Formulation
Reduced Integration
Incompatible Modes
Hybrid
Modified Formulation
Modified/Hybrid
Tri/3, Quad/4, Tri/6, Quad/8
 
 
Tri/6
Tri/6
Options above create CAX3, CAX4, CAX4R, CAX6, CAX6M, CAX8, CAX8R, CAX3H, CAX4H, CAX4RH, CAX6H, CAX6MH, CAX8H, or CAX8RH elements (depending on the selected options and topologies) with SOLID SECTION properties. *ORIENTATION and HOURGLASS STIFFNESS option may also be created, as required. If triangular elements are found where reduced integration is requested, standard integration elements will be used.
Axisymmetric Solid with Twist (General)
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
2D Solid
General Axisymmetric
Standard Formulation
Hybrid
Reduced Integration
Hybrid/Reduced Integration
Tri/3, Quad/4, Tri/6, Quad/8
Quad/4, Quad/8
Options above create CGAX3, CGAX4, CGAX4R, CGAX6, CGAX8, CGAX8R, CGAX3H, CGAX4H, CGAX4RH, CGAX6H, CGAX8H, or CGAX8RH elements (depending on the selected options and topologies) with SOLID SECTION properties. *ORIENTATION and HOURGLASS STIFFNESS options may also be created, as required. If triangular elements are found where reduced integration is requested, standard integration elements will be used.
Membrane
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
Membrane
Standard Formulation
Reduced Integration
 
Tri/3, Quad/4, Tri/6, Quad/8
Options above create M3D3, M3D4, M3D4R, M3D6, M3D8, M3D8R, M3D9 or M3D9R elements (depending on the selected options and topologies) with SOLID SECTION properties. The thickness value on the SOLID SECTION option is included. ORIENTATION and HOURGLASS STIFFNESS options may also be created, as required. If triangular elements are found where reduced integration is requested, standard integration elements will be used.
 
Planar 2D Interface
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
2D Interface
Planar
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No
Separation
Lagrange Vis Damping
Lagrange Vis Damping No
Separation
Quad/4, Quad/8
Options above create INTER2 or INTER3 elements (depending on the selected topology) with INTERFACE, FRICTION, and SURFACE CONTACT properties. The SOFTENED parameter on the SURFACE CONTACT option may be included, depending on the selected option. This element defines an interface region between two portions of a planar model. These elements must be created from one contact surface to the other.
More data input is available for creating Planar 2D Interface elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Description
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option.
Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Press
Defines the pressure at zero clearance. This is the value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the ∗SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
Axisymmetric 2D Interface
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
2D Interface
Axisymmetric
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis DampingNo
Separation
Lagrange Vis Damping
Lagrange Vis Damping No Separation
Quad/4, Quad/8
Options above create INTER2A or INTER3A elements (depending on the selected topology) with *INTERFACE, *FRICTION, and *SURFACE CONTACT properties. The SOFTENED parameter on the *SURFACE CONTACT option may be included, depending on the selected option. This element defines an interface region between two portions of an axisymmetric model. These elements must be created from one contact surface to the other.
More data input is available for creating Axisymmetric 2D Interface elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Description
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option.
Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the *SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points not considered in contact. This is the c value on the ∗SURFACE CONTACT option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient
is constant.
IRS (Shell/Solid)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
IRS (shell/solid)
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No
Separation
Lagrange Vis Damping
Lagrange Vis Damping
No Separation
 
Quad/4
Options above create IRS3, IRS4, and IRS9 elements (depending on the selected topology) with ∗INTERFACE, ∗FRICTION and ∗SURFACE CONTACT properties. The SOFTENED parameter on the ∗SURFACE CONTACT option may be included, depending on the selected option. This defines a rigid surface element for use with solid or shell elements.
More data input is available for creating IRS (shell/solid) elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Description
Reference Node
Reference node common to the IRS elements and the rigid surface.
Friction in Dir_1
Friction in Dir_2
Defines the sliding friction in the element’s 1 and 2 directions. These are the friction coefficients on the second card of the ∗FRICTION option. If Friction in Dir_2 is specified, then the ANISOTROPIC parameter is included on the ∗FRICTION option. These values can be either real constants or references to existing field definitions.
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of , to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option.
Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Press Zero Clearance
Defines the pressure at zero clearance. This is the value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points considered not in contact. This is the c value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient
is constant.
Rigid Surface (Bezier 3D)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
Rigid Surf (Bz3D)
 
 
Quad 4
Options above create a ∗RIGID SURFACE, TYPE=BEZIER option for use in three-dimensional analysis (see Section 7.4.7 of the ABAQUS/Standard User’s manual).
All trias forming up the rigid surface must have the normals pointing towards the contacting surface. Trias must all be connected.
Rigid Surface (LBC)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
Rigid Surface(LBC)
 
 
Quad4,
Tria3
This property set is created when the Rigid-Deform contact lbc is created in the Loads/BCs menu. The creation or deletion of this property set is not required by the user. The elements associated with this property set are translated as R3D3 and R3D4 elements.
2D Rebar
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
Rebar
Cylindrical
General
Standard Formulation
Reduced Integration
Quad/9
Tri/3, Tri/6, Quad/4, Quad/8
Quad/4, Quad/8
The options above create SFM3D3, SFM3D4, SFM3D4R, SFM3D6, SFM3D8, SFM3D8R and SFMCL9 elements (depending on the selected options and topologies) with *SURFACE SECTION properties. The *EMBEDDED ELEMENT and *REBAR LAYER options are also created.
 
Material Name
Defines the material to be used. When entering data here, a list of all isotropic materials in the database is displayed. You can either pick one from the list with the mouse or type in the name. This identifies the material that will be referenced on the *REBAR LAYER option. This property is required.
X-Sectional Area
Defines the area of the rebar cross-section. This is the cross-sectional area value on the *REBAR LAYER option. A real constant, a reference to an existing field definition, or a real list may be entered. A real list is used to specify the cross-sectional area for more than one rebar layer. This property is required.
Spacing
Defines the spacing of the rebars within a layer. This is the spacing value on the *REBAR LAYER option. A real constant, a reference to an existing field definition, or a real list may be entered. A real list is used to specify the spacing for more than one rebar layer. This property is required.
Spacing Unit Type
Defines the unit type for the spacing values. When “Angle” is specified, the ANGULAR SPACING parameter is used for the *REBAR LAYER option. “Distance” is the default value. This property is not required.
Rebar Orient. Angle
Defines the angular orientation of the rebar from the local 1-direction in degrees. This is the angular orientation value on the *REBAR LAYER option. A real constant, a reference to an existing field definition, or a real list may be entered. A real list is used to specify the angular orientation for more than one rebar layer. This property is required.
Host Property Set
Defines the element property set of the elements that host the rebar elements. This is the “HOST ELSET” parameter on the *EMBEDDED ELEMENT option. A reference to an existing element property set may be specified. By default, the solver determines the host elements based on the position of the embedded elements within the model. This property is not required.
Roundoff Tolerance
Defines the value below which the weigh factors of the host element’s nodes will be zeroed out. This is the ROUNDOFF TOLERANCE parameter on the *EMBEDDED ELEMENT option. A real scalar may be specified. The default value is 1E+6. This property is not required.
Orientation System
Defines a local coordinate system for orienting the rebars. This is a reference to an existing coordinate system. The referenced coordinate system defines the data used to create an *ORIENTATION option. The orientation name is then used for the ORIENTATION parameter on the *REBAR LAYER option. This property is not required.
Orientation Axis
Defines the axis of rotation on the “Orientation System” to use for the additional rotation specified by the “Orientation Angle”. The axis should have a nonzero component in the direction of the normal to the surface. An integer value between 1 and 3 may be specified. The local 1-direction is the default value. This property is not required.
Orientation Angle
Defines the additional rotation in degrees about the “Orientation Axis” of the “Orientation System”. Either a real scalar or a reference to an existing field definition may be specified. The default value is zero. This property is not required.
Plane Strain Gasket
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
2D Gasket
Plane Strain
Gasket Behavior Model
Quad4
These options create GKPE4 elements. The *GASKET SECTION option is used to define the gasket thickness, out-of-plane thickness, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the transverse shear behavior.
 
Membrane Material
This property defines the membrane material to be used. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to MEMBRANE. The Elastic Modulus and Poisson's Ratio may vary with temperature. This property is not required.
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
P vs Closure (Loading)
This property defines the pressure versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
P vs Closure (Unloading)
This property defines the pressure versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Shear Stiffness
This property defines the shear stiffness of the gasket elements. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to TRANSVERSE SHEAR. A real constant or a non-spatial field may be used to define this property. The non-spatial fields that have been created with the "Tabular Input" method may be used to define shear stiffness that varies with temperature. This property is not required.
Thickness
This property defines the out-of-plane thickness of the of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Plane Strain Gasket (Material)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
2D Gasket
Plane Strain
Built-in Material
Quad4
These options create GKPE4 elements. The *GASKET SECTION option is used to define the gasket thickness, out-of-plane thickness, initial gap and initial void values. The gasket material is specified using the MATERIAL parameter on the *GASKET SECTION option.
 
Material Name
This property defines the material to be used. It is translated to the ABAQUS input file as the MATERIAL parameter on the *GASKET SECTION option. This property is required.
Thickness
This property defines the out-of-plane thickness of the of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Plane Stress Gasket
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
2D Gasket
Plane Stress
Gasket Behavior Model
Quad4
These options create GKPS4 elements. The *GASKET SECTION option is used to define the gasket thickness, out-of-plane thickness, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the transverse shear behavior.
 
Membrane Material
This property defines the membrane material to be used. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to MEMBRANE. The Elastic Modulus and Poisson's Ratio may vary with temperature. This property is not required.
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
P vs Closure (Loading)
This property defines the pressure versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
P vs Closure (Unloading)
This property defines the pressure versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Shear Stiffness
This property defines the shear stiffness of the gasket elements. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to TRANSVERSE SHEAR. A real constant or a non-spatial field may be used to define this property. The non-spatial fields that have been created with the "Tabular Input" method may be used to define shear stiffness that varies with temperature. This property is not required.
Thickness
This property defines the out-of-plane thickness of the of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Plane Stress Gasket (Thick only)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
2D Gasket
Plane Stress
Thickness Behavior Only
Quad4
These options create GKPS4N elements. The *GASKET SECTION option is used to define the gasket thickness, out-of-plane thickness, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction.
 
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
P vs Closure (Loading)
This property defines the pressure versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
P vs Closure (Unloading)
This property defines the pressure versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Thickness
This property defines the out-of-plane thickness of the of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Plane Stress Gasket (Material)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
2D Gasket
Plane Stress
Built-in Material
Quad4
These options create GKPS4 elements. The *GASKET SECTION option is used to define the gasket thickness, out-of-plane thickness, initial gap and initial void values. The gasket material is specified using the MATERIAL parameter on the *GASKET SECTION option.
 
Material Name
This property defines the material to be used. It is translated to the ABAQUS input file as the MATERIAL parameter on the *GASKET SECTION option. This property is required.
Thickness
This property defines the out-of-plane thickness of the of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Axisymmetric Gasket
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
2D Gasket
Axisymmetric
Gasket Behavior Model
Quad4
These options create GKAX4 elements. The *GASKET SECTION option is used to define the gasket thickness, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the transverse shear behavior.
 
Membrane Material
This property defines the membrane material to be used. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to MEMBRANE. The Elastic Modulus and Poisson's Ratio may vary with temperature. This property is not required.
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
P vs Closure (Loading)
This property defines the pressure versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
P vs Closure (Unloading)
This property defines the pressure versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Shear Stiffness
This property defines the shear stiffness of the gasket elements. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to TRANSVERSE SHEAR. A real constant or a non-spatial field may be used to define this property. The non-spatial fields that have been created with the "Tabular Input" method may be used to define shear stiffness that varies with temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Axisymmetric Gasket (Thick only)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
2D Gasket
Axisymmetric
Thickness Behavior Only
Quad4
These options create GKAX4N elements. The *GASKET SECTION option is used to define the gasket thickness, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction.
 
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
P vs Closure (Loading)
This property defines the pressure versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
P vs Closure (Unloading)
This property defines the pressure versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
 
Axisymmetric Gasket (Material)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
2D Gasket
Axisymmetric
Built-in Material
Quad4
These options create GKAX4 elements. The *GASKET SECTION option is used to define the gasket thickness, initial gap and initial void values. The gasket material is specified using the MATERIAL parameter on the *GASKET SECTION option.
 
Material Name
This property defines the material to be used. It is translated to the ABAQUS input file as the MATERIAL parameter on the *GASKET SECTION option. This property is required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
3D Line Gaske
t
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
2D Gasket
Line
Gasket Behavior Model
Quad4
These options create GK3D4L elements. The *GASKET SECTION option is used to define the gasket thickness, width, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the transverse shear behavior.
 
Membrane Material
This property defines the membrane material to be used. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to MEMBRANE. The Elastic Modulus and Poisson's Ratio may vary with temperature. This property is not required.
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
F/L vs. Closure (Loading)
This property defines the force per unit length versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
F/L vs. Closure (Unloading)
This property defines the force per unit length versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Shear Stiffness
This property defines the shear stiffness of the gasket elements. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to TRANSVERSE SHEAR. A real constant or a non-spatial field may be used to define this property. The non-spatial fields that have been created with the "Tabular Input" method may be used to define shear stiffness that varies with temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Width
This property defines the width of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
3D Line Gasket (Thick only)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
2D Gasket
Line
Thickness Behavior Only
Quad4
These options create GK3D4LN elements. The *GASKET SECTION option is used to define the gasket thickness, width, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction.
 
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
F/L vs. Closure (Loading)
This property defines the force per unit length versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
F/L vs. Closure (Unloading)
This property defines the force per unit length versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Width
This property defines the width of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
3D Line Gasket (Material)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
2D
2D Gasket
Line
Built-in Material
Quad4
These options create GK3D4L elements. The *GASKET SECTION option is used to define the gasket thickness, width, initial gap and initial void values. The gasket material is specified using the MATERIAL parameter on the *GASKET SECTION option.
 
Material Name
This property defines the material to be used. It is translated to the ABAQUS input file as the MATERIAL parameter on the *GASKET SECTION option. This property is required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Width
This property defines the width of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Solid
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
3D
Solid
Standard Formulation
Hybrid
Hybrid/Reduced Integration
Reduced Integration
Incompatible Modes
Hybrid/Incompatible Modes
Modified Formulation
Modified/Hybrid
Laminate
 
Tet/4, Tet/10, Wedge/6, Wedge/15, Hex/8, Hex/20, Hex/27
 
 
 
Tet/10
Tet/10
Options above create C3D4, C3D6, C3D8, C3D8R, C3D10, C3D10M, C3D15, C3D20, C3D20R, C3D4H, C3D6H, C3D8H, C3D8RH, C3D10H, C3D10MH, C3D15H, C3D20H, C3D20RH, C3D27, C3D27R, C3D27H, or C3D27RH elements (depending on the selected options and topologies) with SOLID SECTION properties. ORIENTATION and HOURGLASS STIFFNESS options may also be created, as required. If tetrahedral or wedge elements are found where reduced integration is requested, standard integration elements will be used.
 
Material Name
Defines the material to be used. When entering data, a list of all materials in the database is displayed. You can either pick one from the list with the mouse or type the name in. This identifies the material which will be referenced on the *SOLID SECTION option. This property is required.
Orientation Axis
This property defines the the orientation of the material within the shell element. This is a reference to an existing coordinate system. The referenced coordinate system defines the data used to create the *ORIENTATION option.
Stack Direction
This property defines the direction in which the material layers are stacked. This is the STACK DIRECTION parameter on the *SOLID SECTION option. An integer value of 1, 2 or 3 may be entered. Please see the section on defining composite solid elements in the ABAQUS Standard User’s Manual to determine the correct stack direction. This property is not required. The default value is 3.
3D Interface
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
3D
3D Interface
Elastic Slip Soft Contact
Elastic Slip Hard Contact
Lagrange Soft Contact
Lagrange Hard Contact
Elastic Slip No Separation
Lagrange No Separation
Elastic Slip Vis Damping
Elastic Slip Vis Damping No Separation
Lagrange Vis Damping
Lagrange Vis Damping No Separation
 
Hex/8, Hex/20, Hex/27
Options above create INTER4, INTER8 or INTER9 elements (depending on the selected topology) with *INTERFACE, *FRICTION, and *SURFACE CONTACT properties. The SOFTENED parameter on the *SURFACE CONTACT option may be included, depending on the selected option. This element defines an interface region between two portions of a spatial model. These elements must be created from one contact surface to the other.
More data input is available for creating 3D Interface elements by scrolling down the input properties menu bar on the previous page. Listed below are the remaining options contained in this menu. Elastic Slip, Slip Tolerance, and No Sliding Contact are mutually exclusive. If values are entered for more than one of these options, all but the first will be ignored.
Property Name
Description
Elastic Slip
Defines the absolute magnitude of the allowable maximum elastic slip to be used in the stiffness method for sticking friction. This is the value of the ELASTIC SLIP parameter on the ∗FRICTION option.
Slip Tolerance
Defines the value of to redefine the ratio of allowable maximum elastic slip to characteristic element length dimension. The default is .005. This is the value of the SLIP TOLERANCE parameter on the ∗FRICTION option.
Stiffness in Stick
This is currently not used.
Maximum Friction Stress
Defines the equivalent shear stress limit of the gap element. This is the value of the TAUMAX parameter on the ∗FRICTION option.
Clearance Zero Pressure
Defines the clearance at which the contact pressure is 0. This is the c value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Pressure Zero Clearance
Defines the pressure at zero clearance. This is the value on the ∗SURFACE CONTACT, SOFTENED option. This property is only used for the Soft Contact option. This is a real constant.
Maximum Overclosure
Defines the maximum overclosure allowed in points considered not in contact. This is the c value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
Maximum Negative Pressure
Defines the magnitude of the maximum negative pressure allowed to be carried across points in contact. This is the value on the ∗SURFACE CONTACT option. This property is only used for the Hard Contact option. This is a real constant.
No Sliding Contact
Chooses the Language multiplier formulation for sticking friction when completely rough (no slip) friction is desired.
Clearance Zero Damping
Clearance at which the damping coefficient is zero.
Damping Zero Clearance
Damping coefficient at zero clearance.
Frac Clearance Const Damping
Fraction of the clearance interval over which the damping coefficient is constant.
Thermal Link
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Thermal
1D
Link
 
 
Bar/2, Bar/3
Options above create DC1D2 or DC1D3 elements, depending on the specified topology with *SOLID SECTION properties. The cross-sectional area value on the *SOLID SECTION option is included.
Thermal Axisymmetric Shell
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Thermal
1D
Axisymmetric Shell
Homogeneous
 
Bar/2, Bar/3
Options above create DSAX1 or DSAX2 elements (depending on the specified topology) with *SHELL SECTION properties.
Thermal Axisymmetric Shell (Laminated)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Thermal
1D
Axisymmetric Shell
Laminate
 
Bar/2, Bar/3
Options above create DSAX1 or DSAX2 elements (depending on the specified topology) with SHELL SECTION, COMPOSITE properties.
Thermal 1D Interface
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Thermal
1D
1D Interface
 
 
Bar/2
Options above create DINTER1 elements with INTERFACE properties. These elements must be created from one contact surface to the other. ∗GAP CONDUCTANCE and ∗GAP RADIATION options are also created, as required.
Thermal Shell
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Thermal
2D
Shell
Homogeneous
 
Quad/4, Quad/8
Options above create DS3, DS4, DS6 or DS8 elements (depending on the selected topology) with *SHELL SECTION properties. An *ORIENTATION option may also be created, as required.
Thermal Shell (Laminated)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Thermal
2D
Shell
Laminate
 
Quad/4, Quad/8
Options above create DS3, DS4, DS6 or DS8 elements (depending on the selected topology) with *SHELL SECTION, COMPOSITE properties. An *ORIENTATION option may also be created, as required.
Thermal Planar Solid
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Thermal
2D
2D Solid
Planar
Axisymmetric
Standard Formulation
Convection/Diffusion
Convection/Diffusion w/Dispersion Control
Tri/3, Quad/4, Quad/8
Quad/4
Quad/4
Options above create DC2D3, DC2D4, DC2D6, DC2D8, DCC2D4, DCC2D4D, DCAX3, DCAX4, DCAX6, DCAX8,DCCAX4, or DCCAX4D elements (depending on the selected options and topologies) with SOLID SECTION properties. The thickness value on the SOLID SECTION option is included. An ORIENTATION option may also be created, as required.
Thermal Preference (Planar)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Thermal
2D
2D Interface
Planar
Axisymmetric
 
Quad/4, Quad/8
Options above create DINTER2, DINTER3, DINTER2A, or DINTER3A elements (depending on the selected option and topology) with *INTERFACE properties. These elements must be created from one contact surface to the other. *GAP CONDUCTANCE and ∗GAP RADIATION options are created, as required.
 
Thermal Solid
 
Analysis Type
Dimension
Type
Option 1
Topologies
Thermal
3D
Solid
Standard Formulation
Convection/Diffusion
Convection/Diffusion w/ Dispersion Control
Tet/4, Tet/10, Wedge/6, Wedge/15, Hex/8, Hex/20
Hex/8
Options above create DC3D4, DC3D6, DC3D8, DC3D10, DC3D15, DC3D20, DCC3D8, or DCC3D8D (depending on the selected options and topologies) elements with *SOLID SECTION properties. An *ORIENTATION option may also be created, as required.
Thermal Preference (Solid)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Thermal
3D
3D Interface
 
 
Hex/8, Hex/20
Options above create DINTER4 or DINTER8 elements (depending on the selected) with *INTERFACE properties. These elements must be created from one contact surface to the other. *GAP CONDUCTANCE and ∗GAP RADIATION options are also created, as required.
Solid Gasket
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
3D
Gasket
Gasket Behavior Model
 
Wedge6, Hex8
These options create GK3D8 or GK3D6 elements depending on the element topology. The *GASKET SECTION option is used to define the gasket thickness, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the transverse shear behavior.
 
Membrane Material
This property defines the membrane material to be used. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to MEMBRANE. The Elastic Modulus and Poisson's Ratio may vary with temperature. This property is not required.
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
P vs Closure (Loading)
This property defines the pressure versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
P vs Closure (Unloading)
This property defines the pressure versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Shear Stiffness
This property defines the shear stiffness of the gasket elements. It is translated to the ABAQUS input file as the *GASKET ELASTICITY option with the COMPONENT parameter set to TRANSVERSE SHEAR. A real constant or a non-spatial field may be used to define this property. The non-spatial fields that have been created with the "Tabular Input" method may be used to define shear stiffness that varies with temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Orientation System
This property defines the coordinate system to use in defining the local two and three directions for the gasket elements. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. An existing coordinate frame may be used to define this property. This property is not required.
Orientation Axis
This property defines the axis of rotation of the Orientation System for the Orientation Angle. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. An integer value of 1, 2 or 3 may be used to define this property. This property is not required. The default value is 1.
Orientation Angle
This property defines the additional rotation about the Orientation Axis in degrees. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Solid Gasket (Thick only)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
3D
Gasket
Thickness Behavior Only
 
Wedge6, Hex8
These options create GK3D8N or GK3D6N elements depending on the element topology. The *GASKET SECTION option is used to define the gasket thickness, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the
thickness direction.
 
Behavior Type
This property defines the type of behavior for the thickness direction. It may be set to either "Damage" or "Elastic-Plastic". This value is translated to the ABAQUS input file as the TYPE parameter on the *GASKET THICKNESS BEHAVIOR option. This property is required.
P vs Closure (Loading)
This property defines the pressure versus gasket closure for loading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to LOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either Displacement or Displacement and Temperature. This property is required.
P vs Closure (Unloading)
This property defines the pressure versus gasket closure for unloading in the thickness direction. It is translated to the ABAQUS input file as the *GASKET THICKNESS BEHAVIOR option with the DIRECTION parameter set to UNLOADING. A non-spatial field created with the "Tabular Input" method must be used to define this property. The field's independent variables must be either displacement or displacement and temperature. This property is not required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Solid Gasket (Material)
 
Analysis Type
Dimension
Type
Option 1
Option 2
Topologies
Structural
3D
Gasket
Built-in Material
 
Wedge6, Hex8
These options create GK3D8 or GK3D6 elements depending on the element topology. The *GASKET SECTION option is used to define the gasket thickness, initial gap and initial void values. The *GASKET THICKNESS BEHAVIOR option is used to define the behavior in the thickness direction. The *GASKET ELASTICITY option is used to define the transverse shear behavior.
 
Material Name
This property defines the material to be used. It is translated to the ABAQUS input file as the MATERIAL parameter on the *GASKET SECTION option. This property is required.
Gasket Thickness
This property defines the thickness of the gasket elements. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required. When this property is not specified, the gasket elements' thicknesses are determined from their nodal coordinates.
Thickness Direction
This property defines the thickness direction (local one direction) for the elements. It is translated to the ABAQUS input file on the *GASKET SECTION option. A real vector or a spatially varying vector field may be used to define this property. This property is not required.
Orientation System
This property defines the coordinate system to use in defining the local two and three directions for the gasket elements. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. An existing coordinate frame may be used to define this property. This property is not required.
Orientation Axis
This property defines the axis of rotation of the Orientation System for the Orientation Angle. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. An integer value of 1, 2 or 3 may be used to define this property. This property is not required. The default value is 1.
Orientation Angle
This property defines the additional rotation about the Orientation Axis in degrees. It is translated to the ABAQUS input file as an *ORIENTATION option that is referenced in the *GASKET SECTION option from the ORIENTATION parameter. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Gap
This property defines the initial gap in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.
Initial Void
This property defines the initial void in the thickness direction of the gasket element. It is translated to the ABAQUS input file as an entry on the *GASKET SECTION option. A real constant or a spatially varying field may be used to define this property. This property is not required.