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 | |
• 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 | 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 | |||
• 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 DampingNo Separation Lagrange Vis Damping Lagrange Vis Damping No Separation | GAPUNI | ||
Axisym Shell | • Laminate | 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) | • 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 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 | |||
• Membrane | 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 |
Dimension | Type | Option 1 | Option 2 | Name |
1D | • Link | DCID2, DCID3 | ||
Axisymmetric Shell | • Laminate | DSAX1, DSAX2 | ||
DINTER1 | ||||
2D | Shell | • Laminate | 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 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 0D | Mass | Point/1 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 0D | Rotary Inertia | Point/1 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 0D | Grounded Spring | Linear | Point/1 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 0D | Grounded Spring | Nonlinear | Point/1 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 0D | Grounded Damper | Linear | Point/1 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 0D | Grounded Damper | Nonlinear | Point/1 |
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 |
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. |
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 |
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. |
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 |
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. |
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 |
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. |
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 |
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 | 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. |
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. |
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 |
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 | 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. |
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 |
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 | 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. |
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 |
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. |
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 |
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 | 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. |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Truss | Standard Formulation Hybrid | Bar/2. Bar/3 Bar/2. Bar/3 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Spring | Linear | Standard Formulation | Bar/2 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Spring | Linear | Fixed Direction | Bar/2 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Spring | Nonlinear | Standard Formulation | Bar/2 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Spring | Nonlinear | Fixed Direction | Bar/2 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Damper | Linear | Standard Formulation | Bar/2 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Damper | Linear | Fixed Direction | Bar/2 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Damper | Nonlinear | Standard Formulation | Bar/2 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Damper | Nonlinear | Fixed Direction | Bar/2 |
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 |
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 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Axisymmetric Shell | Homogeneous | Bar/2 Bar/3 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Axisymmetric Shell | Laminate | Bar/2 |
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 |
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. |
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 |
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. |
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 |
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. |
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 |
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. |
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 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Slide Line | Bar/2, Bar/3 |
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 |
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. |
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 |
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. |
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 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Rigid Surf (Seg) | Bar/2 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Rigid Surf (Cyl) | Bar/2 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Rigid Surf (Axi) | Bar/2 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Rigid Surf (Bz2D) | Bar/2 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Rigid Line(LBC) | Bar/2 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Rebar | Axisymmetric General Axisymmetric | Bar/2, Bar/3 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (2D Model) | ALIGN | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (2D Model) | AXIAL | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (2D Model) | BEAM | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (2D Model) | CARTESIAN | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (2D Model) | JOIN | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (2D Model) | JOINTC | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (2D Model) | LINK | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (2D Model) | ROTATION | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (2D Model) | SLOT | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (2D Model) | TRANSLATOR | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (2D Model) | WELD | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (3D Model) | ALIGN | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (3D Model) | AXIAL | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (3D Model) | BEAM | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (3D Model) | CARDAN | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (3D Model) | CARTESIAN | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (3D Model) | CONSTANT VELOCITY | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (3D Model) | CVJOINT | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (3D Model) | CYLINDRICAL | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (3D Model) | EULER | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (3D Model) | FLEXION-TORSION | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (3D Model) | HINGE | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (3D Model) | JOIN | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (3D Model) | JOINTC | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (3D Model) | LINK | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (3D Model) | PLANAR | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (3D Model) | RADIAL-THRUST | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (3D Model) | REVOLUTE | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (3D Model) | ROTATION | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (3D Model) | SLIDE-PLANE | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (3D Model) | SLOT | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (3D Model) | TRANSLATOR | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (3D Model) | UJOINT | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (3D Model) | UNIVERSAL | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | Mech Joint (3D Model) | WELD | Bar/2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | 1D Gasket | Axisymmetric Link | Gasket Behavior Model | Bar2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | 1D Gasket | Axisymmetric Link | Thickness Behavior Only | Bar2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | 1D Gasket | Axisymmetric Link | Built-in Material | Bar2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | 1D Gasket | 3D Link | Gasket Behavior Model | Bar2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | 1D Gasket | 3D Link | Thickness Behavior Only | Bar2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | 1D Gasket | 3D Link | Built-in Material | Bar2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | 1D Gasket | 2D Link | Gasket Behavior Model | Bar2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | 1D Gasket | 2D Link | Thickness Behavior Only | Bar2 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 1D | 1D Gasket | 2D Link | Built-in Material | Bar2 |
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. |
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 |
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. |
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 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 2D | Shell | Thick Shell | Homogeneous | Tri/3, Quad/4, Tri/6, Quad/8 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 2D | Shell | Thick Shell | Laminate | Tri/3, Quad/4, Tri/6, Quad/8 |
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 |
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. |
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 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 2D | Shell | General Thick Shell | Tri/3, Quad/4, Tri/6, Quad/8 |
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. |
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 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 2D | Shell | Large Strain Shell | Tri/3, Quad/4, Tri/6, Quad/8 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 2D | Shell | General Large Strain Shell | Tri/3, Quad/4 |
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. |
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 |
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 |
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. |
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 |
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 |
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 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 2D | Membrane | Standard Formulation Reduced Integration | Tri/3, Quad/4, Tri/6, Quad/8 |
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 |
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. |
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 |
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. |
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 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 2D | Rigid Surf (Bz3D) | Quad 4 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 2D | Rigid Surface(LBC) | Quad4, Tria3 |
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 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 2D | 2D Gasket | Plane Strain | Gasket Behavior Model | Quad4 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 2D | 2D Gasket | Plane Strain | Built-in Material | Quad4 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 2D | 2D Gasket | Plane Stress | Gasket Behavior Model | Quad4 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 2D | 2D Gasket | Plane Stress | Thickness Behavior Only | Quad4 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 2D | 2D Gasket | Plane Stress | Built-in Material | Quad4 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 2D | 2D Gasket | Axisymmetric | Gasket Behavior Model | Quad4 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 2D | 2D Gasket | Axisymmetric | Thickness Behavior Only | Quad4 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 2D | 2D Gasket | Axisymmetric | Built-in Material | Quad4 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 2D | 2D Gasket | Line | Gasket Behavior Model | Quad4 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 2D | 2D Gasket | Line | Thickness Behavior Only | Quad4 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 2D | 2D Gasket | Line | Built-in Material | Quad4 |
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. |
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 |
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. |
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 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Thermal | 1D | Link | Bar/2, Bar/3 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Thermal | 1D | Axisymmetric Shell | Homogeneous | Bar/2, Bar/3 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Thermal | 1D | Axisymmetric Shell | Laminate | Bar/2, Bar/3 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Thermal | 1D | 1D Interface | Bar/2 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Thermal | 2D | Shell | Homogeneous | Quad/4, Quad/8 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Thermal | 2D | Shell | Laminate | Quad/4, Quad/8 |
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 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Thermal | 2D | 2D Interface | Planar Axisymmetric | Quad/4, Quad/8 |
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 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Thermal | 3D | 3D Interface | Hex/8, Hex/20 |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 3D | Gasket | Gasket Behavior Model | Wedge6, Hex8 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 3D | Gasket | Thickness Behavior Only | Wedge6, Hex8 |
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. |
Analysis Type | Dimension | Type | Option 1 | Option 2 | Topologies |
Structural | 3D | Gasket | Built-in Material | Wedge6, Hex8 |
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. |