Element Properties

Ansys > Building A Model > Element Properties

XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">

Element Properties

The Element Properties form appears when the Element Properties toggle, located on the Patran main form, is chosen. When creating an element property several options are available. The selections made on these forms will determine which Element Properties form will appear, and ultimately, which ANSYS element will be created.

The following page gives an introduction to the Element Properties form, followed by definitions of the element properties supported by the Patran ANSYS Application Preference.

Element Properties Form

This form appears when Element Properties is selected on the main form. Four option menus are used to determine which ANSYS element types will be created, and which property forms will be displayed. The individual property forms are explained later in this section. For more information on the Element Properties form, see Create Element Property Sets (p. 62) in the Patran Reference Manual.

The following table outlines the options when the Analysis Type is set to Structural There is more information on the Element Property input forms following the tables


Dimension	Type	Option 1	Option 2
0D	• Mass	• UX,UY • UX,UY,UZ • UX,UY,RZ, • UX,UY,UZ,RX,RY,RZ



1D	• Beam	• General Section • Curved w/Pipe Section • Pipe Section • Tapered Section
	• Planar Spar
	• Spar
	• Spring/Damper	• Standard Formulation • Fixed Direction
	• Spring/Damper	• Standard Formulation • Fixed Direction
	• Gap
	• Planar Gap
	• Cable
	• Combination
	• Axisym Shell
	• Planar Beam	• General Section • Circular Section • General Plastic Section • Pipe Section • Rectangular Section • Tapered Section
2D	• Thin Shell	• Homogeneous • Laminate
	• Thick Shell	• Homogeneous • Laminate
	Bending Panel
	• 2D Solid	• Plane Strain • Plane Stress • Axisymmetric
	• Membrane
	• Shear Panel
	• Twist Panel
	• 2D Coupled Field Solid	• Plane Strain • Plane Stress • Axisymmetric
3D	• Solid	• Homogeneous	• Standard Formulation • Rotational DOF
3D	• Solid	• Laminate
	• Coupled Field Solid	• Voltage • Magnetic Flux • UX,UY,UZ • UX,UY,UZ,Temp, Volt,Mag Flux

The following table outlines the options when the Analysis Type is set to Thermal.There is more information on the Element Properties input forms following this table


Dimension	Type	Option 1	Option 2
0D	• Mass
1D	• Link	• 3D	Conduction Convection Radiation


		• 2D Link
	• Spring/Damper
	• Combination
	• Thermal - Electric Link
2D	• Shell
	• 2D Solid	• Planar • Axisymmetric
	• Thermal - Electric 2D Solid	• Planar • Axisymmetric
	• 2D Coupled Field Solid	• Temperature • Magnetic Flux
3D	• Solid
	• Thermal - Electric Solid
	• Coupled Field Solid

Structural Mass (MASS21)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	0D	Mass	UX, UY UX, UY, UZ	Point/1

Use this form to create the MASS21 (Generalized Mass) elements. KEYOPT(3) is defined by the selection of option 1 to be either 2, or 4. When UX,UY is selected, KEYOPT(3) is set to 4. When UX,UY,UZ is selected KEYOPT(3) is set to 2.

2D Structural Mass with Rotation

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	0D	Mass	UX, UY, RZ	Point/1

Use this form to create the MASS21 (Generalized Mass) elements. KEYOPT(3) is set to 3.

3D Structural Mass with Rotation

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	0D	Mass	UX, UY, UZ, RX, RY, RZ	Point/1

Use this form to create the MASS21 (Generalized Mass) elements. KEYOPT(3) is set to 0.

3D Elastic Beam (BEAM4)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	1D	Beam	General Section	Bar/2

Use this form to create the BEAM4 (Three-Dimensional Elastic Beam) elements.

This is a list of data input, available for creating the 3D elastic Beam (BEAM4) which were not shown on the previous page. Use the scroll bars to view these properties.


Property Name	Description
Theta	Theta defines an additional rotation from the beam Orientation data. After the beam orientation is initially established using the Beam Orientation Def data, the Theta rotation is made around the local X-axis to define the final local coordinate system. This is the THETA real constant. This value can either be a real scalar or a reference to an existing field definition. This property is optional.
Initial Strain	Initial Strain defines the initial strain built into the element. This is the INITIAL STRAIN real constant. This value can either be a real scalar or a reference to an existing field definition. This property is optional.
Ixx	Ixx defines the torsional moment of inertia about the local x-axis. This is the IXX real constant. This value can either be a real scalar, or a reference to an existing field definition. This property is optional.
Z Shear Constant Y Shear Constant	Z and Y Shear Constants are the ratios of the actual beam cross-sectional area to the effective area resisting shear deformation in the Z and Y directions. These are the SHEARZ and SHEARY real constants. These values can either be real scalars or references to existing field definitions. These properties are optional.
Z Shear Constant Y Shear Constant
Mass Matrix Option	Mass Matrix Option defines the type of mass matrix to be used for these elements. This defines the setting of KEYOPT(1). This value is a character string, which can be set either to consistent, or reduced. This property is optional. However, if it is not defined, consistent will be assumed.
Node Location Option	Node Location Option defines the setting of KEYOPT(3). This defines how the beam is oriented with respect to the nodes. This value can be set to origin of Y-Z axes, centroid, or shear center. This property is optional.

Curved Pipe (Elbow) (PIPE18)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	1D	Beam	Curved Pipe (Elbow) (PIPE18)	Bar/2

Use this form to create the PIPE18 (Elastic Curved Pipe (Elbow)) elements


Note:	Results translation is supported for ANSYS Revision 5 only.

This is a list of data input, available for creating the Curved Pipe (Elbow) (PIPE18) which were not shown on the previous page. Use the scroll bars to view these properties.


Property Name	Description
[Strs Intns. Factor @ 1]	Define the stress intensity factor at end I and end J of the beam. These are the SIFI and SIFJ real constants. These properties are optional.
[Flexibility]	Defines the flexibility factor. This is the FLEX real constant. This property is optional.
[Internal Fluid Density]	Defines the density of the fluid contained in the pipe. This is the DENSFL real constant. This property is optional.
[Ext Insulation Density]	Defines the density of the external insulation applied to the pipe. This is the DENSIN real constant. This property is optional.
[Ext Insulation Thick]	Defines the thickness of the external insulation. This is the TKIN real constant. This property is optional.
[Ext Insulation Thick]
[Corrosion Thick Allow]	Defines the allowable thickness of the corrosion on the pipe. This is the TKCORR real constant. This property is optional.
[Temp Gradient Defn]	Defines the representation of the temperature gradient. This is KEYOPT(1). The value is a character string which can be set to either “THRU_WALL” or “DIAMETRAL”. The KEYOPT will be set to 0 or 1 respectively. This is an optional property.
[Pipe Flex Factor Type]	Defines the type of flexibility factor to be used if the FLEX real constant is not specified. This is KEYOPT(3). The value is a character string which may to set to “ANSYS NO PRESS TERM”, “ANSYS WITH PRESS TERM”, or “KARMAN”. These correspond to KEYOPT settings of 0, 1, and 2. This property is optional.
[Member Results Print]	Specifies if member forces are to be printed. This is KEYOPT(6). The value is a character string which may be set to either “NO MEMBER PRINTOUT” or “PRNT MBR FORCE & MOMENT”. These correspond to KEYOPT settings of 0 and 2. This is an optional property.

Elastic Straight Pipe (PIPE16)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	1D	Beam	Elastic Straight Pipe (PIPE16)	Bar/2

Use this form to create the PIPE16 (Elastic Straight Pipe) elements.


Note:	Results translation is supported for ANSYS Revision 5 only.

This is a list of data input, available for creating the Curved Pipe (Elbow) (PIPE18) which were not shown on the previous page. Use the scroll bars to view these properties.


Property Name	Description
Flexibility	Defines the flexibility factor. This is the FLEX real constant. This property is optional.
[Internal Fluid Density]	Defines the density of the fluid contained in the pipe. This is the DENSFL real constant. This property is optional.
[Ext Insulation Density]	Defines the density of the external insulation applied to the pipe. This is the DENSIN real constant. This property is optional.
[Ext Insulation Thick]	Defines the thickness of the external insulation. This is the TKIN real constant. This property is optional.
[Corrosion Thick Allow]	Defines the allowable thickness of the corrosion on the pipe. This is the TKCORR real constant. This property is optional.
[Insulation Surf area]	Defines the surface area of the insulation applied to the pipe. This is the AREAIN real constant. This property is optional.
[Pipe Wall Mass]	Overrides the pipe wall mass calculation if a value is specified. This is the MWALL real constant. This property is optional.
[Pipe Axial Stiffness]	Overrides the pipe stiffness calculation if a value is specified. This is the STIFF real constant. This is an optional property.
[Pipe Rotordynamic Spin]	Defines the value of the rotordynamic spin. This is the SPIN real constant. This property is optional.
[Temp Gradient Defn]	Defines the representation of the temperature gradient. This is KEYOPT(1). The value is a character string which can be set to either “THRU_WALL” or “DIAMETRAL”. The KEYOPT will be set to 0 or 1 respectively. This is an optional property.
[Strs Intens Factr Defn]	Defines which stress intensification factor(s) will be used. This is KEYOPT(2). The value is a character string which can be set to “FROM SIFI & SIFJ”, “NODE I TEE JOINT CALC,“, “NODE J TEE JOINT CALC”, or “BOTH NODES TEE JNT CALC”. These correspond to KEYOPT settings of 0, 1, 2, or 3. This is an optional property.
[Pipe Element Type]	Defines what type of pipe element this will represent. This is KEYOPT(4). The value is a character string which can be set to “STRAIGHT PIPE”, “VALVE”, “REDUCER”, “FLANGE”, “EXPANSION JOINT”, “MITERED BEND”, or “TEE BRANCH”. These correspond to KEYOPT settings of 0. 1. 2. 3. 4. 5. or 6. This is an optional property.
[Pipe Press Component]	Defines which component(s) of pressure are to be used. This is KEYOPT(5). The value is a character string which may be set to either “NORMAL COMPONENT”, or “FULL PRESSURE”. These correspond to KEYOPT settings of 0 or 1. This is an optional property.
[Member Results Print]	Specifies if member forces are to be printed. This is KEYOPT(6). The value is a character string which may be set to either “NO MEMBER PRINTOUT” or “PRNT MBR FORCE & MOMENT”. These correspond to KEYOPT settings of 0 and 2. This is an optional property.
[Gyro Damping Matrix]	Specifies if a gyroscopic damping matrix is to be calculated. This is KEYOPT(7). The value is a character string which may be set to either “NO GYRO DAMP MATRIX”, or “COMPUTE GYRO DAMP MATRIX”. These correspond to KEYOPT settings of 0 or 1. If a gyroscopic damping matrix is to be computed, the SPIN real constant must be greater than zero and DENSFL and DENSIN must be zero.

Tapered Unsymmetrical Beam (BEAM44)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	1D	Beam	Tapered Section	Bar/2

Use this form to create the BEAM44 (3D Tapered Unsymmetrical Beam) elements.

This is a list of data input, available for creating the Tapered Unsymmetrical Beam (BEAM44) which were not shown on the previous page. Use the scroll bars to view these properties.


Property Name	Description
Area at End J	Area at End J defines the cross-sectional area at each end of the element. These are the AREA1 and AREA2 real constants. This value can either be a real scalar or a reference to an existing field definition. This property is required.
Z Inertia at J Y Inertia at J	Defines the area moments of inertia about the Z and Y axes. These are the IZ2 and IY2 real constants. These values can either be real scalars or reference to existing field definitions. These properties are optional.
Z Bottom Thickness at J Y Bottom Thickness at J	Z and Y Bottom Thickness defines the distances from the center of gravity of the beam cross-section to the outermost fibers at the bottom of the element in the Z direction at End J. These values are the TKZB2, and TKYB2 real constants. These values are real scalars and are optional properties.
Torsional Inertia @ I Torsional Inertia @ J	Torsional Inertia defines the torsional inertia values at the ends of the beam. These are IX1 and IX2 real constants. These values can either be real scalars or references to existing field definitions, and are optional properties.
Nodal Offset at I Nodal Offset at J	Nodal Offset defines the distance from the nodes to the actual center of gravity of the section at each end of the beam. These are the DX1, DY1, DZ1, DX2, DY2, and DZ2 real constants. These values are real vectors, and are optional properties.
Z Shear Constant Y Shear Constant	Z and Y Shear Constant are the ratios of the actual beam cross-sectional area to the effective and resisting shear deformation in the Z and Y directions. These are the SHEARZ and SHEARY real constants. These values can either be real scalars or references to existing field definitions, and are optional properties.
Z Top Thickness at I, J Y Top Thickness at I, J	Z and Y Top Thickness defines the distances from the center of gravity of the beam cross-section to the outermost fibers in the positive and negative y and z directions at either end of the element. These values are the TKZT1, TKYT1, TKZT2 and TKYT2 real constants. These values are real scalars and are optional properties.
Z Dir Shear Area at I, J Y Dir Shear Area at I, J	Z and Y Dir Shear Areas define the shear areas in the y and z directions at either end of the beam. These are the AREAZ1, AREAZ2, and ARESY2 real constants. These values can either be real scalars or references to existing field definitions, and are optional properties.



Torsional Shear at I Torsional Shear at J	Torsional Shear defines the torsional stress factors at either ends of the beam. These are used in calculating the torsional stresses in the element. These are the TSF1 and TSF2 real constants. These values can either be real scalars or references to existing field definitions, and are optional properties.
Z Shr Ctr Offset at I, J Y Shr Ctr Offset at I, J	Z and Y Shr Ctr Offset defines the offset from the center of gravity of the section to the shear center. These are the DSCZ1, DSCY1, DSCZ2, and DSCY2 real constants. These values can either be real scalars or references to existing field definitions, and are optional properties. If any of these are defined, KEYOPT(5) will be increased to 3.
Z Shr Ctr Offset at I, J Y Shr Ctr Offset at I, J
Z Elast Found Stiffness Y Elast Found Stiffness	Z and Y Elast Found Stiffness defines the elastic foundation stiffness in the z and y directions. These are defined as the pressure required to produce a unit normal deflection of the foundation. These are the EFSZ and EFSY real constants. These values can either be real scalars or referenced to existing field definitions, and are optional properties. If either of these properties are defined, KEYOPT(5) will be increased to 3.
Mass Matrix Options	Mass Matrix Option defines the type of mass matrix to be used for these elements. This defines the setting of KEYOPT(1). This value is a character string, which can be set to either constant, or lumped, and is an optional property. However, if it is not defined, consistent will be assumed.
End I Releases End J Releases	End Release defines the end release conditions at either end of the element. These define the settings of KEYOPTs (3) and (4). These values are character strings, which can be set to NONE, RX, RY, RZ, RX&RY, or RX&RY&RZ. These properties are optional.

2D Spar (LINK1)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	1D	Planar Spar		Bar/2

Use this form to create the LINK1 (Two-Dimensional Spar) elements.

3D Spar (LINK8)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	1D	Spar		Bar/2

Use this form to create the LINK8 (Three-Dimensional Spar) elements.

Spring-Damper Axial (COMBIN14)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	1D	Spring/Damper	Standard Formulation	Bar/2

Use this form to create the COMBIN14 (Spring-Damper) elements.

Spring-Damper Fixed (COMBIN14)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	1D	Spring/Damper	Fixed Direction	Bar/2

Use this form to create the COMBIN14 (Spring-Damper) elements.

3D Point-Point Contact

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	1D	Gap		Bar/2

Use this form to create the CONTAC52 (Three-Dimensional Preference) elements.

2D Point-Point Contact

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	1D	Planar Gap		Bar/2

Use this form to create the CONTAC12 (Two-Dimensional Preference) elements.

This is a list of data input, available for creating the 2D Point-Point Contact, which were not shown on the previous page. Use the scroll bars to view these properties.


Property Name	Description
Sticking Options	Defines what stiffness is to be used for the Sticking Stiffness. This defines the setting of KEYOPT(1). This value can either be set to use sticking stiffness or zero sticking stiffness. If use sticking stiffness is selected, the KS real constant is used to define the sticking stiffness. If not specified, ANSYS will default to the KEYOPT setting, corresponding to use sticking stiffness. This is an optional property.
Gap Size Option	Defines how the initial gap opening is defined. This defines the setting of KEYOPT(4). This value can either be based on gap size value, or based on node locations. This is an optional property. However, if not specified, base on gap size value will be assumed.

Cable (LINK10)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	1D	Cable		Bar/2

Use this form to create the LINK10 (Cable) elements.


Note:	Results translation is supported for ANSYS Revision 5 only.

Combination (COMBIN40)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	1D	Combination		Bar/2

Use this form to create the COMBIN40 (Combination) elements.

This is a list of data input, available for creating the Combination (COMBIN 40), which were not shown on the previous page. Use the scroll bars to view these properties.


Property Name	Description
Degree(s)-of-freedom	Defines which degree-of-freedom this element is attached to. This defines the setting of KEYOPTs (2) and (3). This value can be set to ux, uy, uz, rotx, roty, or rotz. This is a required property.
Mass Distribution	Defines the placement of the element mass values. This defines the setting of KEYOPT(6). This value can be set to, at node I, at node J, or equally distributed. This is an optional property. However, if it is not specified, at node I will be assumed.
Lock up Option	Removes the gap opening capability once the gap has closed. This defines the setting of KEYOPT(1). Allowable options are: Include, and Do Not Include. This is an optional property.

Axisymmetric Shell (SHELL51)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	1D	Axisymmetric Shell		Bar/2

Use this form to create the SHELL51(Axisymmetric Structural Shell) elements.


Note:	Results translation is supported for ANSYS Revision 5 only.

2D Elastic Beam (BEAM3)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	1D	Planar Beam	General Section	Bar/2

Use this form to create the BEAM3 (Two-Dimensional Elastic Beam) elements.

2D Beam-Circular Section (BEAM 23)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	1D	Planar Beam	Circular Section	Bar/2

Use this form to create the BEAM23 (2D plastic beam) elements with a circular cross section


Note:	Results translation is supported for ANSYS Revision 5 only.

2D Beam-General Sect (BEAM 23)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	1D	Planar Beam	General Plastic Section	Bar/2

Use this form to create the BEAM23 (2D Plastic Beam) elements with a general beam section.


Note:	Results translation is supported for ANSYS Revision 5 only.

This is a list of data input, available for creating the 2D Beam General Section, which were not shown on the previous page. Use the scroll bars to view these properties.


Property Name	Description
Wt Factor@ L(-50)	Defines the area weighting factors for the numerical integration of cross-sectional properties. These are the A(-50), A(-30), A(0), A(30), and A(50) real constants. These are required properties. For more information on these area factors, see <bold_helvetica>Figure 2-1.
[Z shear Constant]	Defines the shear deflection constant. This is the SHEARZ real constant. This is an optional property.
[Shear Option]	Specifies if shear deflection is to be included. This is KEYOPT(2). The value is a character string which may be set to “NO SHEAR DEFLECTION,” or “INCLUDE SHEAR DEFLECTION.” These correspond to KEYOPT values of either 0 or 1. This is an optional property.
[Member Results Print]	Specifies if member forces are to be printed. This is KEYOPT(6). The value is a character string which may be set to either “NO MEMBER PRINTOUT” or “PRNT MBR FORCE & MOMENT.” These correspond to KEYOPT settings of 0 and 2. This is an optional property.

Figure 2‑1 Weighting Factors for General Section (KEYOPT6=4)


Important:	L(i) are weighting factors for the numerical integration of cross-sectional properties such as area and moment of inertia. For further information on how to define the L(i) see the ANSYS Users Manual, Volume III, Elements and Volume IV, Theory, for the BEAM23 element.

2D Beam-Pipe Section (BEAM 23)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	1D	Planar Beam	Pipe Section	Bar/2

Use this form to create the BEAM23 (2D Plastic Beam) element with a Pipe cross section.


Note:	Results translation is supported for ANSYS Revision 5 only.

2D Beam-Rectangular Section (BEAM 23)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	1D	Planar Beam	Rectangular Section	Bar/2

Use this form to create the BEAM23 (2D Plastic Beam) elements with a rectangular cross section.


Note:	Results translation is supported for ANSYS Revision 5 only.

2D Elastic Tapered Unsymmetric Beam (BEAM 54)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	1D	Planar Beam	Tapered Section	Bar/2

Use this form to create the BEAM54(2D Elastic Tapered Unsymmetric Beam) elements.


Note:	Results translation is supported for ANSYS Revision 5 only.

This is a list of data input available for creating the 2D Elastic Tapered Unsymmetrical Beam (BEAM54) which were not shown on the previous page. Use the scroll bars to view these properties.


Parameter Name	Description
Z Inertia at J	Defines the area moment of inertia about the principal axis of the beam at end J. This is the IZ2 real constant and is an optional property.
Dist. C.G. to Top at J Dist C.G. to Bot at J	Defines the distance from the center of gravity to the top and bottom of the beam at end J. These are the HYT2 and HYB2 real constants and are optional properties.
Nodal Offset at I Nodal Offset at J	Nodal Offset defines the distance from the nodes to the actual center of gravity of the section at each end of the beam. These are the DX1, DY1, DX2, and DY2 real constants. These values are real vectors, and are optional properties.
Z Shear Constant	Defines the shear deflection constant. This is the SHEARZ real constant. It is an optional property.
Shear Area at I Shear Area at J	Defines the shear areas at either end of the beam. These are the AREAS1, and AREAS2 real constants. These values can either be real scalars or references to existing field definitions, and are optional properties.
Elast Found Stiffness	Defines the elastic foundation stiffness. This is the EFS real constant and is an optional property.

Elastic Shell (SHELL63)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	2D	Thin Shell	Homogeneous	Tri/3, Quad/4

This form creates the SHELL63 (Elastic Quadrilateral Shell) elements. KEYOPT(1) is set to 0 to indicate both bending and membrane stiffness.

This is a list of data input, available for creating the Elastic Shell (SHELL 63), which were not shown on the previous page. Use the scroll bars to view these properties.


Property Name	Description
Dist C.G to Top Dist C.G. to Bottom	Defines the section height from the neutral plane to the top of bottom fiber for computing bending stresses. These are the CTOP and CBOT real constants. These values can either be real scalars or references to existing field definitions. These are optional properties.
Extra Shapes Option	Indicates whether extra displacement shapes are to be used in the element formulation. This defines the setting of KEYOPT(3). This value can be set to, INCLUDE, or DO NOT INCLUDE. This is an optional property.
Pressure Load Options	Defines how distributed loads are represented within the element. This defines the setting to KEYOPT(6). This can be set to REDUCED or CONSISTENT This is an optional property. However, if it is not specified, REDUCED will be assumed.
Mass Matrix Options	Defines the type of mass matrix to be used for these elements. This defines the setting of KEYOPT(7). This value is a charter string, which can be set to either CONSISTENT, LUMPED, or REDUCED. This is an optional property. However, if it is not defined, REDUCED will be assumed.

100-Layer Structural Shell

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	2D	Thin Shell	Laminate	Tri⁄6, Quad⁄8

Use this form to create the SHELL99 (8-Node Layered Shell) elements.

Structural Shell (SHELL43/93)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	2D	Thick Shell	Homogeneous	Tri⁄3, Quad⁄4 Tri⁄6, Quad⁄8

Use this form to create the SHELL43 (Plastic Quadrilateral Shell) or SHELL93 (8-Node Isoparametric Shell) elements, depending on the selected topology.

16-Layer Structural Shell

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	2D	Thick Shell	Laminate	Tri⁄6, Quad⁄8

Use this form to create the SHELL91 (8-Node Layered Shell) elements.

Bending Panel (SHELL63)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	2D	Bending Panel		Tri⁄3, Quad⁄4

Use this form to create the SHELL63 (Elastic Quadrilateral Shell) elements. KEYOPT(1) is set to 2 to indicate bending stiffness only.

This is a list of data input, available for creating the Bending Panel (SHELL63), which were not shown on the previous page. Use the scroll bars to view these properties.


Property Name	Description
[Bending Inertia Ratio]	Defines the ratio of the bending moment of inertia to be used to that calculated from the input thickness. This is the RMI real constant. This value can either be a real scalar or a reference to an existing field definition. This is an optional property.
Dist C.G to Top Dist C.G. to Bottom	Defines the section height from the neutral plane to the top of bottom fiber for computing bending stresses. These are the CTOP and CBOT real constants. These values can either be real scalars or references to existing field definitions. These are optional properties.
Extra Shapes Option	Indicates whether extra displacement shapes are to be used in the element formulation. This defines the setting of KEYOPT(3). This value can be set to INCLUDE, or DO NOT INCLUDE. This is an optional property.
Pressure Load Options	Defines how distributed loads are represented within the element. This defines the setting to KEYOPT(6). This can be set to REDUCED or CONSISTENT. This is an optional property. However, if it is not specified, REDUCED will be assumed.
Mass Matrix Options	Defines the type of mass matrix to be used for these elements. This defines the setting of KEYOPT(7). This value is a character string, which can be set to either CONSISTENT or REDUCED. This is an optional property. However, if it is not defined, Reduced will be assumed.

2D Plane Solid

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	2D	2D Solid	Plane Strain Axisymmetric	Tri⁄3, Quad⁄4 Tri⁄6, Quad⁄8

Use this form to create either the PLANE2 (2-D, 6-Node Triangular Solid), the PLANE42 (2D Isoparametric Solid), or the PLANE82 (2-D, 8-Node Isoparametric Solid) elements, which depends on the selected topology. KEYOPT(3) is set to define either axisymmetric or plane strain behavior, depending on the selection for option 1.

2D Plane Stress Solid

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	2D	2D Solid	Plane Stress	Tri⁄3, Quad⁄4 Tri⁄6, Quad⁄8

Membrane Shell (SHELL41)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	2D	Membrane		Tri/3, Quad/4

Use this form to create the SHELL41(Membrane Shell) elements.


Note:	Results translation is supported for ANSYS Revision 5 only.

This is a list of data input available for creating the Membrane Shell (SHELL41) which were not shown on the previous page. Use the scroll bars to view these properties.


Parameter Name	Description
Elastic Found Stiffness	Defines the elastic foundation stiffness. This is defined as the pressure required to produce a unit normal deflection of the foundation. This is the EFS real constant. This value can either be a real scalar or a reference to an existing field definition. This is an optional property.
Stiffness Dir Options	Defines the stiffness behavior of the element to specify if the element has stiffness in both tension and compression or if it has stiffness only in tension and will collapse in compression. This defines the setting of KEYOPT(1). This is a optional property.
Extra Shapes Option	Indicates whether extra displacement shapes are to be used in the element formulation. This defines the setting of KEYOPT(3). This value can be set to INCLUDE or DO NOT INCLUDE. This is an optional property.

Shear Panel (SHELL28)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	2D	Shear Panel		Quad⁄4

Use this form to create the SHELL28 (4-Node Quadrilateral Shear⁄Twist Panel) elements.

Twist Panel (SHELL28)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	2D	Twist Panel		Quad⁄4

Use this form to create the SHELL28 (4-Node Quadrilateral Shear⁄Twist Panel) elements.

2D Plane Coupled Field Solid

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option 1	Option 2	Topologies
Structural	2D	2D Coupled Field Solid	Plane Strain Plane Stress Axisymmetric	Magnetic Flux UX, UY UX,UY,Temp,Mag Flux Volt, Mag Flux UX,UY,Volt	Tri/3, Quad/4

Use this form to create the PLANE13 (2D Coupled-Field Solid) elements. KEYOPT(3) will be set appropriately to specify if the element is plane strain, plane stress, or axisymmetric, depending upon the selection for Option 1. KEYOPT(1) will be set depending on the selection for Option 2.


Note:	Results translation is supported for ANSYS Revision 5 only.

Structural Solid

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	3D	Solid	Homogeneous Standard Formulation	Tet⁄4, Wedge⁄6, Hex⁄8, Tet⁄10, Wedge⁄15, Hex⁄20

Use this form to create the SOLID45 (3D Isoparametric Solid), SOLID92 (3D Tetrahedral Structural Solid), or the SOLID95 (3D Structural Solid) elements.

Structural Solid with Rotations

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	3D	Solid	Homogeneous Rotational DOF	Tet/4, Wedge/6, Hex/8

Use this form to create the SOLID72 (4-Node Tetrahedral Structural Solid with Rotations) or the SOLID73 (3D 8-Node Structural Solid with Rotations) elements.


Note:	Results translation is supported for ANSYS Revision 5 only.

Layered Structural Solid

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	3D	Solid	Laminate	Tet⁄4, Wedge⁄6, Hex⁄8

Use this form to create the SOLID46 (8-Node Layered Solid) elements.

Coupled Field Solid

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Structural	2D	Coupled Field Solid	Voltage Magnetic Flux UX,UY,UZ UX,UY,UZ, Temp, Volt,Mag Flux	Tet⁄4, Wedge⁄6, Hex⁄8, Tet⁄10, Wedge⁄15, Hex⁄20

Use this form to create the SOLID98 (Tetrahedral Coupled-Field Solid) or the SOLID5 (3D Coupled Field Solid) depending upon the selected topology. KEYOPT(1) will be set depending upon the selection of Option.


Note:	Results translation is supported for ANSYS Revision 5 only.

Thermal Mass (MASS71)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Thermal	0D	Mass		Point⁄1

Use this form to create the MASS71 (Lumped Thermal Mass with Variable Heat Generation) elements.

Conduction Bar (LINK33)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option 1	Option 2	Topologies
Thermal	1D	Link	3D Link	Conduction	Bar⁄2

Use this form to create the LINK33 (3-Dimensional Heat Conduction Bar) elements.

Convection Link (LINK34)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option 1	Option 2	Topologies
Thermal	1D	Link	3D Link	Convection	Bar⁄2

This form creates the LINK34 (Convection Link) elements.

Radiation Link (LINK31)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option 1	Option 2	Topologies
Thermal	1D	Link	3D Link	Radiation	Bar⁄2

Use this form to create the LINK31 (Radiation Link) elements.

Conduction Bar (LINK32)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Thermal	1D	Link	2D Link	Bar⁄2

Use this form to create the LINK32 (2-Dimensional Heat Conduction) Bar.

Thermal Spring-Damper (COMBIN14)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Thermal	1D	Spring/Damper		Bar⁄2

Use this form to create the COMBIN14 (Spring-Damper) elements with KEYOPT(2) set for a TEMP degree-of-freedom.

Thermal Combination (COMBIN40)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Thermal	1D	Combination		Bar⁄2

Use this form to create the COMBIN40 (Combination) elements with KEYOPT(3) set to 8 for a TEMP degree-of-freedom.

Thermal Electric Link (LINK 68)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Thermal	1D	Electric Link		Bar⁄2

Use this form to create the LINK68 (Thermal-Electric Line) elements.


Note:	Results translation is supported for ANSYS Revision 5 only.

Thermal Shell (SHELL57)

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Thermal	2D	Shell		Tri⁄3, Quad⁄4

Use this form to create the SHELL57 (Isoparametric Quadrilateral Thermal Shell) elements.

2D Planar Thermal Solid

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Thermal	2D	2D Solid	Planar	Tri⁄3, Quad⁄4, Tri⁄6, Quad⁄8

Use this form to create the PLANE35 (2-D, 6-Node Triangular Thermal Solid), PLANE55 (2D Isoparametric Thermal Solid), or the PLANE77 (2-D, 8-Node Isoparametric Thermal Solid) element with KEYOPT (3) set for Planar behavior.

2D Axisymmetric Thermal Solid

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Thermal	2D	2D Solid	Axisymmetric	Tri⁄3, Quad⁄4 Tri⁄6, Quad⁄8

Thermal Electric 2D Solid

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Thermal	2D	Electric 2D Solid	Planar, Axisymmetric	Tri/3, Quad/4

Use this form to create the PLANE67 (2D Thermal-Electric Solid) elements.


Note:	Results translation is supported for ANSYS Revision 5 only.

2D Coupled Field Solid

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Thermal	2D	2D Coupled Field Solid	Temperature Magnetic Flux	Tri/3, Quad/4

Use this form to create the PLANE13 (2D Coupled Field Solid) elements. KEYOPT(1) will be set depending on the selection of the option.


Note:	Results translation is supported for ANSYS Revision 5 only.

3D Thermal Solid

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Thermal	3D	Solid		Tet⁄4, Wedge⁄6, Hex⁄8, Tet⁄10, Wedge⁄15, Hex⁄20

Use this form to create the SOLID70 (Isoparametric Thermal Solid), SOLID87 (10-Node Tetrahedral Thermal Solid), or SOLID90 (3-D, 20-Node Isoparametric Thermal Solid) elements, which depend on the selected topology.

3D Thermal - Electric Solid

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Thermal	3D	Electric Solid		Tet⁄4, Wedge⁄6, Hex⁄8, Tet⁄10, Wedge⁄15, Hex⁄20

Use this form to create the SOLID69 (3D Thermal-Electric Solid) elements.


Note:	Results translation is supported for ANSYS Revision 5 only.

3D Thermal Coupled Field Solid

This form appears when the Input Properties button is selected on the Element Properties form when the following is applied.


Analysis Type	Dimension	Type	Option(s)	Topologies
Thermal	3D	Coupled Field Solid	Temperature, Voltage, Magnetic Flux, UX,UY,UZ,Temp, Volt, Mag Flux Temp, Volt, Mag Flux	Tet⁄4, Wedge⁄6, Hex⁄8, Tet⁄10, Wedge⁄15, Hex⁄20

Use this form to create the SOLID98 (Tetrahedral Coupled-Field Solid) or SOLID5 (3D Coupled-Field Solid) elements depending on the selected topology. KEYOPT(1) will be set depending on the selection of the option.


Note:	Results translation is supported for ANSYS Revision 5 only.