Element Properties

MSC Nastran > Building A Model > 2.7 Element Properties

XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">

2.7 Element Properties

The Element Properties form appears when the Element Properties toggle, located on the Patran main form, is chosen.There are several option menus available when creating element properties. The selections made on the Element Properties menu will determine which element property form appears, and ultimately, which MD Nastran element will be created.

The following pages give an introduction to the Element Properties form, and details of all the element property definitions supported by the Patran MD Nastran Preference.

Element Properties Form

This form appears when Element Properties is selected on the main menu. There are four option menus on this form. Each will determine which MD Nastran element type will be created and which property forms will appear. The individual property forms are documented later in this section. For a full description of this form, see Element Properties Forms (p. 61) in the Patran Reference Manual.

The following table outlines the option menus when Analysis Type is set to Structural.

Table 2‑1
Dimension	Type	Option 1	Option 2
0D	• Mass	• Coupled • Grounded • Lumped


	• Grounded Spring
	• Grounded Damper
	• Grounded Bush
1D	• Beam	• General Section	• Standard • P-Formulation





		• Curved w/General Section
		• Curved w/Pipe Section
		• Lumped Section
		• Tapered Section	• Standard • P-element
		• General Section Beam (CBEAM)
	• Rod	• General Section	• Standard • CONROD
	• Rod	• General Section	• Standard • CONROD
		• Pipe Section
	• Spring
	• Damper	• Scalar • Viscous
	• Damper	• Scalar • Viscous
	• Gap	• Adaptive • Non-Adaptive
	• 1D Mass
	• PLOTEL
	• Bush
	• Spot Weld Connector
	• Fastener Connector
2D	• Shell	• Homogeneous	• Standard • Revised • P-element





		• Laminate	• Standard • Revised
		• Equivalent Section	• Standard • Revised • P-element
		• Field Point Mesh (exterior acoustic element)
	• Bending Panel	• Standard • Revised • P-element
	• Bending Panel	• Standard • Revised • P-element
	• 2D-Solid	• Plane Strain	• Standard • Revised • P-Formulation • Hyperelastic Formulation
		• Plane Stress
		• Axisymmetric	• Standard • Hyperelastic Formulation • PLPLANE
		• Infinite (exterior acoustic element)
	• Membrane	• Standard • Revised • P-Formulation
	• Membrane	• Standard • Revised • P-Formulation
	• Shear Panel
3D	• Solid	• Homogeneous	• Standard • P-Formulation • Hyperelastic Formulation • Solid Shell
3D	• Solid	• Homogeneous
		• Laminate • Gasket

Coupled Point Mass (CONM1)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	0D	Mass	Coupled	Point/1

Use this form to create a CONM1 element. This defines a 6 x 6 symmetric mass matrix at a geometric point of the structural model.

This is a list of Input Properties available for creating a CONM1 element that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties.


Prop Name	Description
Mass Component 3,3 Mass Component 4,1 Mass Component 4,2 Mass Component 4,4 Mass Component 5,1 Mass Component 5,2 Mass Component 5,3 Mass Component 5,4 Mass Component 5,5 Mass Component 6,1 Mass Component 6,2 Mass Component 6,3 Mass Component 6,4 Mass Component 6,5 Mass Component 6,6	Defines the values of the mass matrix. These are the Mij fields on the CONM1 entry. These properties can either be real values or references to existing field definitions. Each of these properties are optional; however, at least one must be defined.

Grounded Scalar Mass (CMASS1)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	0D	Mass	Grounded	Point/1

Use this form to create a CMASS1 element and a PMASS property. This defines a scalar mass element of the structural model. Only one node is used in this method, and the other node is defined to be grounded.

Lumped Point Mass (CONM2)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	0D	Mass	Lumped	Point/1

Use this form to create a CONM2 element. This defines a concentrated mass at a geometric point of the structural model.

This is a list of Input Properties available for creating a CONM2 element that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties.


Prop Name	Description
Inertia 3,1 Inertia 3,2 Inertia 3,3	Inertia i,j defines the rotation inertia properties of this lumped mass. These are the Iij fields on the CONM2 entry. These values can be either real values or references to existing field definitions. These values are optional.

Grounded Scalar Spring (CELAS1/CELAS1D)

This subordinate form appears when the Input Properties button is selected on the Element Properties form when the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	0D	Grounded Spring		Point/1

Use this form to create a CELAS1 or CELAS1D (for SOL 700) element and a PELAS property. This defines a scalar spring element of the structural model. Only one node is used in this method. The other node is defined to be grounded.

Grounded Scalar Damper (CDAMP1/CDAMP1D)

This subordinate form appears when the Input Properties button is selected on the Element Properties form when the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	0D	Grounded Damper		Point/1

Use this form to create a CDAMP1 or CDAMP1D (for SOL 700) element and a PDAMP property. This defines a scalar damper element of the structural model. Only one node is used in this method. The other node is defined to be grounded.

Bush

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	1D	Bush		Bar/2

This is a list of Input Properties available. Use the menu scroll bar on the Input Properties form to view these properties.


Prop Name	Description
Bush Orientation System	CID specifies the Grounded Bush Orientation System. The element X,Y, and Z axes are aligned with the coordinate system principal axes. If the CID is for a cylindrical or spherical coordinate system, the grid point specified locates the system. If CID = 0, the basic coordinate system is used.
Spring Constant 1 Spring Constant 2 Spring Constant 3 Spring Constant 4 Spring Constant 5 Spring Constant 6 Stiff. Freq Depend 1 Stiff. Freq Depend 2 Stiff. Freq Depend 3 Stiff. Freq Depend 4 Stiff. Freq Depend 5 Stiff. Freq Depend 6	Defines the stiffness associated with a particular degree of freedom. This property is defined in terms of force per unit displacement and can be either a real value or a reference to an existing field definition for defining stiffness vs. frequency.
Stiff. Force/Disp 1 Stiff. Force/Disp 2 Stiff. Force/Disp 3 Stiff. Force/Disp 4 Stiff. Force/Disp 5 Stiff. Force/Disp 6	Defines the nonlinear force/displacement curves for each degree of freedom of the spring-damper system.
Damping Coefficient 1 Damping Coefficient 2 Damping Coefficient 3 Damping Coefficient 4 Damping Coefficient 5 Damping Coefficient 6 Damp. Freq Depend 1 Damp. Freq Depend 2 Damp. Freq Depend 3 Damp. Freq Depend 4 Damp. Freq Depend 5 Damp. Freq Depend 6	Defines the force per velocity damping value for each degree of freedom. This property can be either a real value or a reference to an existing field definition for defining damping vs. frequency
Structural Damping Struc. Damp Freq Depend	Defines the non-dimensional structural damping coefficient (GE1). This property can be either a real value, or a reference to an existing field definition for defining damping vs. frequency.
Stress Recovery Translation Stress Recovery Rotation	Stress recovery coefficients. The element stress are computed by multiplying the stress coefficients with the recovered element forces.
Strain Recovery Translation Strain Recovery Rotation	Strain Recovery Coefficients. The element strains are computed by multiplying the strain coefficients with the recovered element strains.

General Section Beam (CBAR)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	1D	Beam	General Section	Bar/2

Use this form to create a CBAR element and a PBAR or PBARL property. A CBARAO entry will be generated if any Station Distances are specified. This defines a simple beam element in the structural model.


Note:	CBAR entries will include all user input pin flags.


Section Name	Specifies a beam section previously created using the beam library
• Value Type	Allows you to define a bar/beam section either by Dimensions (PBARL/PBEAML) or by Properties (PBAR/PBEAM). If Dimensions is choosen, the MD Nastran’s built-in section library (Version 69 and later), PBARL/PBEAML, (for the standard Beam Library) or PBRSECT/PBMSECT (for an Arbitrary section) will be used to define the bar/beam. If Properties is chosen, the standard bar/beam properties, PBAR/PBEAM will be used to define the beam section. If the Dimensions Option is set to Dimensions, the Translation Parameters Version must be set to version 69 or later.
Material Name	Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse, or type in the name. This property defines the value to be used in the MID field on the PBAR entry. This property is required.
Bar Orientation	Defines the local element coordinate system to be used for any cross-sectional properties. This orientation will define the local XY plane, where the x-axis is along the beam. This orientation defines the value for the X1, X2, X3, or G0 fields on the CBAR entry. This property is required.
• Value Type	Specifies how the bar orientation is defined: Vector – Specified using a vector Node Id – Specified using an existing node in the beam XY plane When the value type is Vector, it is always input in either the Patran global or some other Patran user defined coordinate system (i.e. <0 1 0 Coord 5>).
• Reference Coordinates	Specifies the MD Nastran coordinate system in which the bar orientation vector will be written to the CBAR entry: Analysis - Displacement Coordinate System at GA Coord 0 - Basic Coordinate System If Analysis is specified, a G will be written to the first position of the OFFT value on the CBAR entry. If Coord 0 is specified, a B will be written. Note: The reference coordinate system specified does not affect how the input is interpreted within Patran. Only how it is written to the CBAR entry.
Offset @ Node 1 Offset @ Node 2	Defines the offset from the nodes to the actual centroids of the beam cross section. These orientations are defined as vectors. These properties, after any necessary transformations, become the W1A, W2A, W3A, W1B, W2B, and W3B fields on the CBAR entry. These properties are optional.
• Value Type	Specifies how the bar orientation is defined: Vector – Specified using a vector This is the only method available. The Reference Coordinate System controls how the vector input is interpreted in Patran.
• Reference Coordinates	Specifies the MD Nastran coordinate system in which the offset vectors will be written to the CBAR entry and how the vector input will be interpreted in Patran: Analysis - Displacement Coordinate Systems at GA and GB Element - Element Coordinate System If Analysis is specified, a G will be written to the second or third position of the OFFT value on the CBAR entry. Within Patran, the vector will be interpreted to be in either the Patran global or some other Patran user defined coordinate system (i.e. <0 1 0 Coord 5>). If Element is specified, an E will be written to the second or third position of the OFFT value on the CBAR entry. Within Patran, the vector will be interpreted to be in the Element coordinate system.
Pinned DOFs @ Node 1 Pinned DOFs @ Node 2	These degrees of freedom are in the element local coordinate system. Values that can be specified are UX, UY, UZ, RX, RY, RZ, or any combination. These properties are used to remove connections between the node and selected degrees of freedom at the two ends of the beam. This option is commonly used to create a pin connection by specifying RX, RY, and RZ to be released. Defines the setting of the PA and PB fields on the CBAR record. These properties are optional. Note that if pinned DOF releases are defined within a property set, but the end nodes of the beams are connected to beams of a different property set, then no pinned DOFs will be written for those beams (PA or PB will be left blank). To override this and force the pin flags to be written per the property set, use an "" after the specification for the DOFs. (This may be problematic if the property sets defined different pin DOFs.) For example, if rotation about the 2nd DOF is to be freed, specify "RY." These values must be typed into the data box. Although there is a pull down menu next to the data box showing the valid selections, you will have to type the values in if more than one DOF or the "" is to be specified. Specifying the "" by itself does nothing.
Area	Defines the cross-sectional area of the element. This is the A field on the PBAR entry. This value can be either real values or a reference to an existing field definition. This property is required.
Inertia 1,1 Inertia 2,2 Inertia 2,1	Defines the various area moments of inertia of the cross section. These are the I1, I2, and I12 fields on the PBAR entry. These values can be either real values or references to existing field definitions. These values are optional.
Torsional Constant	Defines the torsional stiffness of the beam. This is the J field on the PBAR entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Shear Stiff, Y Shear Stiff, Z	Defines the shear stiffness values. These are the K1 and K2 fields on the PBAR entry. These values can be either real value or references to existing field definitions. This property is optional.
Nonstructural Mass	Defines mass not included in the mass derived from the material of the element. This is defined in terms of mass per unit length of the beam. This is the NSM field on the PBAR entry. This value can be either a real value or reference to an existing field definition. This property is optional.
Y of Point C Z of Point C Y of Point D Z of Point D Y of Point E Z of Point E Y of Point F Z of Point F	Indicates the stress recovery. They define the Y and Z coordinates of the stress recovery points across the section of the beam, as defined in the local element coordinate system. These are the C1, C2, D1, D2, E1, E2, F1, and F2 fields on the PBAR entry. These values can be either real values or references to existing field definitions. These properties are optional.
[Contact Beam Radius]	This allows the equivalent radius for beam-to-beam contact to be different for each beam cross section. The MD Nastran entry BCBMRAD is written to the .bdf file. The BCBMRAD entry format is different for SOL 400 and SOL 600.
[Station Distances]	Defines up to 6 points along each bar element. Values specified are fractions of the beam length. Therefore, these values are in the range of 0. to 1. This defines the X1 and X6 fields on the CBARAO entry. The SCALE field on the CBARAO entry is always set to FR. The alternate format for the CBARAO entry is not supported. These values are real values. These properties are optional.
Create Sections, I C L ..., Beam Library	Activates the Beam Library forms. These forms will allow the user to define beam properties by choosing a standard cross section type and inputing dimensions.

P-Formulation General Beam (CBEAM)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	1D	Beam	General Section P-Formulation	Bar/2, Bar/3 Bar/4

Use this form to create a CBEAM element and a PBEAM or PBEAML property. This form defines a simple beam element in the structural model for an adaptive, p-element analysis.


Note:	.Patran will check the element associativity to other elements sharing this property set and will not export user defined pin unless the user includes an asterisk (*) in the string, in which case Patran will export the defined pin flags for all elements in the property set.

This is a list of Input Properties available for creating a CBEAM element and a PBEAM or PBEAML property that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties.


Prop Name	Description
Area	Defines the cross-sectional area of the element. This is the A field on the PBEAM entry. This value can be either real values or a reference to an existing field definition. This property is required.
Inertia 1,1 Inertia 2,2 Inertia 2,1	Defines the various area moments of inertia of the cross section. These are the I1, I2, and I12 fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These values are optional.
Torsional Constant	Defines the torsional stiffness of the beam. This is the J field on the PBEAM entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Shear Stiff, Y Shear Stiff, Z	Defines the shear stiffness values. These are the K1 and K2 fields on the PBEAM entry. These values can be either real values or references to existing field definitions. This property is optional.
Nonstructural Mass	Defines mass not included in the mass derived from the material of the element. This is defined in terms of mass per unit length of the beam. This is the NSM field on the PBEAM entry. This value can be either a real value or reference to an existing field definition. This property is optional.
Y of Point C Z of Point C X of Point D Y of Point D X of Point E Y of Point E X of Point F Y of Point F	Indicates the stress recovery. Define the Y and Z coordinates of the stress recovery points across the section of the beam as defined in the local element coordinate system. These are the C1, C2, D1, D2, E1, E2, F1, and F2 fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
Station Distances	Defines up to 6 points along each bar element. Values specified are fractions of the beam length. Therefore, these values are in the range of 0. to 1. This defines the X1 and X6 fields on the CBARAO entry. The SCALE field on the CBARAO entry is always set to FR. The alternate format for the CBARAO records is not supported. These values are real values. These properties are optional.
Starting P-orders and Maximum P-orders	Polynomial orders for displacement representation within elements. Each contains a list of three integers referring to the directions defined by the P-order Coordinate System (default elemental). Starting P-orders apply to the first adaptive cycle. The adaptive analysis process will limit the polynomial orders to the values specified in Maximum P-orders. These are the Polyi fields on the PVAL entry.
P-order Coord. System	The two sets of three integer p-orders above refer to the axes of this coordinate system. By default, this system is elemental. This is the CID field on the PVAL entry.
Activate Error Estimate	Flag controlling whether this set of elements participates in the error analysis. This is the ERREST field in the ADAPT entry.
P-order Adaptivity	Controls the particular type of p-order adjustment from adaptive cycle to cycle. This is the TYPE field on the ADAPT entry.
Error Tolerance	The tolerance used to determine if the adaptive analysis is complete. By default, equal to 0.1. This is the ERRTOL field on the ADAPT entry.

Curved General Section Beam (CBEND)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	1D	Beam	Curved w/General Section	Bar/2

Use this form to create a CBEND element and a PBEND property. This form defines a curved beam element of the structural model. The CBEND element has several ways to define the radius of the bend and the orientation of that curvature.This element in Patran always uses the method of defining the center of curvature point (GEOM=1). An alternate property of the Curved Pipe element also exists.

This is a list of Input Properties available for creating a CBEND element and a PBEND property that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties.


Prop Name	Description
Inertia 1,1 Inertia 2,2	Defines the various area moments of inertia of the cross section. These properties are the I1 and I2 fields on the PBEND entry. These values can either be real values or references to existing field definitions. These values are optional.
Torsional Constant	Defines the torsional stiffness of the beam. This is the J field on the PBEND entry. This value can be either a real value, or a reference to an existing field definition. This property is optional.
Shear Stiff, R Shear Stiff, Z	Defines the shear stiffness values. These properties are the K1 and K2 fields on the PBEND entry. These values can be either real values or references to existing field definitions. This property is optional.
Nonstructural Mass	Defines mass not included in the mass derived from the material of the element. This property is defined in terms of mass per unit length of the beam and is the NSM field on the PBEND entry. This value can be either real value or a reference to an existing field definition. This property is optional.
Radial NA Offset	Defines the radial offset of the geometric centroid from the end nodes. Positive values move the centroid of the section towards the center of curvature of the pipe bend. This property is the DELTAN field on the PBEND entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
R of Point C Z of Point C R of Point D Z of Point D R of Point E Z of Point E R of Point F Z of Point F	These properties are for stress recovery. They define the R and Z coordinates of the stress recovery points across the section of the beam, as defined in the local element coordinate system. These properties are the C1, C2, D1, D2, E1, E2, F1 and F2 fields on the PBEND entry. These values can be either real values or references to existing field definitions. These properties are optional.

Curved Pipe Section Beam (CBEND)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	1D	Beam	Curved W/Pipe Section	Bar/2

Use this form to create a CBEND element and a PBEND property. This defines a curved pipe or elbow element of the structural model. The internal pressure is defined as part of the element definition because, for pipe elbows, the internal pressure affects the element stiffness.


Prop Name	Description
Internal Pipe Pressure	Indicates the static pressure inside the pipe elbow. This is the P field on the PBEND entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Nonstructural Mass	Defines mass not included in the mass derived from the material of the element. This property is defined in terms of mass per unit length of the beam and is the NSM field on the PBEND entry. This value can either be a real value or a reference to an existing field definition. This property is optional.
Stress Intensification	Indicates the desired type of stress intensification to be used. This is a character string value. This property is the FSI field on the PBEND entry. Valid settings of this parameter are General, ASME, and Welding Council.

Lumped Area Beam (CBEAM/PBCOMP)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	1D	Beam	Lumped Section	Bar/2

Use this form to create a CBEAM element and a PBCOMP property. This defines a beam element of constant cross section, using a lumped area element formulation.The orientation vector can be defined as either a vector or a reference to an existing node in the XY plane.


Note:	Patran will check the element associativity to other elements sharing this property set and will not export user defined pin unless the user includes an asterisk (*) in the string, in which case Patran will export the defined pin flags for all elements in the property set.


Section Name	Specifies a beam section previously created using the beam library
• Value Type	Allows you to define a bar/beam section either by Dimensions (PBARL/PBEAML) or by Properties (PBAR/PBEAM). If Dimensions is choosen, the MD Nastran’s built-in section library (Version 69 and later), PBARL/PBEAML, will be used to define the bar/beam. If Properties is chosen, the standard bar/beam properties, PBAR/PBEAM will be used to define the beam section. If the Dimensions Option is set to Dimensions, the Translation Parameters Version must be set to version 69 or later.
Material Name	Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse, or type in the name. This defines the setting of the MID field on the PBCOMP entry. This property is required.
Bar Orientation	Defines the local element coordinate system to be used for any cross-sectional properties. This orientation will define the local XY plane, where the x-axis is along the beam. This orientation defines the value for the X1, X2, X3, or G0 fields on the CBAR entry. This property is required.
• Value Type	The orientation vector can be defined as either a vector or a reference to an existing node in the XY plane.
• Reference Coordinates	Analysis - Analysis Coordinate System. Coord 0 - Basic Coordinate System.
Offset @ Node 1 Offset @ Node 2	Defines the offset from the nodes to the actual centroids of the beam cross section. These orientations are defined as vectors. These properties, after any necessary transformations, become the W1A, W2A, W3A, W1B, W2B, and W3B fields on the CBEAM entry. On the CBEAM entry, these values are always in the displacement coordinate system of the node. In Patran, they are either global, or in a system specified such as <0 1 0 Coord 5>. These properties are optional.
• Value Type	Specifies that the offset is defined in terms of a vector.
• Reference Coordinates	Analysis - Analysis Coordinate System. Element - Element Coordinate System.
Pinned DOFs @ Node 1 Pinned DOFs @ Node 2	Indicates whether certain degrees of freedom are to be released. By default, all degrees of freedom can transfer forces at the ends of beams. By releasing specified degrees of freedom, pin or sliding type connections can be created. These degrees-of-freedom are in the element local coordinate system. The values that can be specified here are UX, UY, UZ, RX, RY, RZ, or a combination. These properties define the settings of the PA and PB fields on the CBEAM entry and are optional. Note that if pinned DOF releases are defined within a property set, but the end nodes of the beams are connected to beams of a different property set, then no pinned DOFs will be written for those beams (PA or PB will be left blank). To override this and force the pin flags to be written per the property set, use an "" after the specification for the DOFs. (This may be problematic if the property sets defined different pin DOFs.) For example, if rotation about the 2nd DOF is to be freed, specify "RY." These values must be typed into the data box. Although there is a pull down menu next to the data box showing the valid selections, you will have to type the values in if more than one DOF or the "" is to be specified. Specifying the "" by itself does nothing.
Warp DOF @ Node 1 Warp DOF @ Node 2	Defines a node ID where the warping degree-of-freedom constraints and results will be placed. These must reference existing nodes within the model. They are the SA and SB fields on the CBEAM entry. These properties are optional.
Area	Defines the cross-sectional area of the element. This is the A field on the PBCOMP entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Nonstructural Mass	Defines mass not included in the mass derived from the material of the element. This is defined in terms of mass per unit length of the beam. This is the NSM field on the PBCOMP record. This value can be either a real value or a reference to an existing field definition. This property is optional.
Shear Stiff, Y Shear Stiff, Z	Defines the shear stiffness values. These are the K1 and K2 fields on the PBCOMP entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Y of NSM Z of NSM	Defines the offset from the centroid of the cross section to the location of the nonstructural mass. These values are measured in the beam cross-section coordinate system. These properties are the M1 and M2 fields on the PBCOMP entry. These values can be either real values or references to existing field definitions. These properties are optional.
Symmetry Option	Specifies which type of symmetry is being used to define the lumped areas of the beam cross section. This is a character string parameter. The valid settings are No Symmetry, YZ Symmetry, Y Symmetry, Z Symmetry, or Y=Z Symmetry. This defines the setting of the SECTION field on the PBCOMP entry. This property is optional.
Ys of Lumped Areas Zs of Lumped Areas	Defines the locations of the various lumped areas. These are defined in the cross-sectional coordinate system. These properties define the Yi and Zi fields on the PBCOMP entry. These values are lists of real values. These properties are optional.
Area Factors	Defines the Fraction of the total area to be included in this lumped area. The sum of all area factors for a given section must equal 1.0. If the data provided does not meet this requirement, the values will all be scaled to the corrected value. These properties define the values for the Ci fields on the PBCOMP entry. These values are lists of real values. These properties are optional.

Tapered Beam (CBEAM)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	1D	Beam	Tapered	Bar/2

Use this form to create a CBEAM element and a PBEAM or PBEAML property. This defines a beam element with varying cross sections.


Note:	Patran will check the element associativity to other elements sharing this property set and will not export user defined pin unless the user includes an asterisk (*) in the string, in which case Patran will export the defined pin flags for all elements in the property set.


Section Name	Specifies a beam section previously created using the beam library
• Value Type	Allows you to define a bar/beam section either by Dimensions (PBARL/PBEAML) or by Properties (PBAR/PBEAM). If Dimensions is choosen, the MSC.Nastran’s built-in section library (Version 69 and later), PBARL/PBEAML, will be used to define the bar/beam. If Properties is chosen, the standard bar/beam properties, PBAR/PBEAM will be used to define the beam section. If the Dimensions Option is set to Dimensions, the Translation Parameters Version must be set to version 69 or later.
Material Name	Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse, or type in the name. This defines the setting of the MID field on the PBCOMP entry. This property is required.
Bar Orientation	Defines the local element coordinate system to be used for any cross-sectional properties. This orientation will define the local XY plane, where the x-axis is along the beam. This orientation, after any necessary transformations, defines the value for the X1, X2, X3, or G0 fields on the CBEAM entry. This property is required.
• Value Type	Specifies how the bar orientation is defined: Vector – Specified using a vector Node Id – Specified using an existing node in the beam XY plane When the value type is Vector, it is always input in either the Patran global or some other Patran user defined coordinate system (i.e. <0 1 0 Coord 5>).
• Reference Coordinates	Specifies the MD Nastran coordinate system in which the bar orientation vector will be written to the CBEAM entry: Analysis - Displacement Coordinate System at GA Coord 0 - Basic Coordinate System If Analysis is specified, a G will be written to the first position of the OFFT value on the CBEAM entry. If Coord 0 is specified, a B will be written. Note: The reference coordinate system specified does not affect how the input is interpreted within Patran. Only how it is written to the CBEAM entry.
Offset @ Node 1 Offset @ Node 2	Defines the offset from the nodes to the shear centers of the beam cross section. These orientations are defined as vectors. These properties, after any necessary transformations, become the W1A, W2A, W3A, W1B, W2B, and W3B fields on the CBEAM entry. These properties are optional.
• Value Type	Specifies how the bar orientation is defined: Vector – Specified using a vector This is the only method available. The Reference Coordinate System controls how the vector input is interpreted in Patran.
• Reference Coordinates	Specifies the MD Nastran coordinate system in which the offset vectors will be written to the CBEAM entry and how the vector input will be interpreted in Patran: Analysis - Displacement Coordinate Systems at GA and GB Element - Element Coordinate System If Analysis is specified, a G will be written to the second or third position of the OFFT value on the CBEAM entry. Within Patran, the vector will be interpreted to be in either the Patran global or some other Patran user defined coordinate system (i.e. <0 1 0 Coord 5>). If Element is specified, an E will be written to the second or third position of the OFFT value on the CBEAM entry. Within Patran, the vector will be interpreted to be in the Element coordinate system.
Pinned DOFs @ Node 1 Pinned DOFs @ Node 2	Indicates whether certain degrees of freedom are to be released. By default, all degrees of freedom can transfer forces at the ends of beams. By releasing specified degrees of freedom, pin or sliding type connections can be created. These degrees-of-freedom are in the element local coordinate system. The values that can be specified here are UX, UY, UZ, RX, RY, RZ, or a combination. These properties define the settings of the PA and PB fields on the CBEAM entry and are optional. Note that if pinned DOF releases are defined within a property set, but the end nodes of the beams are connected to beams of a different property set, then no pinned DOFs will be written for those beams (PA or PB will be left blank). To override this and force the pin flags to be written per the property set, use an "" after the specification for the DOFs. (This may be problematic if the property sets defined different pin DOFs.) For example, if rotation about the 2nd DOF is to be freed, specify "RY." These values must be typed into the data box. Although there is a pull down menu next to the data box showing the valid selections, you will have to type the values in if more than one DOF or the "" is to be specified. Specifying the "" by itself does nothing.
Warp DOF @ Node 1 Warp DOF @ Node 2	Defines a node ID where the warping degree of freedom constraints and results will be placed. These must reference existing nodes within the model. These are the SA and SB fields on the CBEAM entry. These properties are optional.
Station Distances	Defines stations along each beam element where the section properties will be defined. The values specified here are fractions of the beam length. These values, therefore, are in the range of 0. to 1. These values define the settings of the X/XB fields on the PBEAM record. These values are real values. These properties are optional.
Cross-Sect. Areas	Defines the cross-sectional area of the element. This property defines the settings of the A fields on the PBEAM record. This value can be either a real value, or reference to an existing field definition. This property is required.
Inertias 1,1 Inertias 2,2 Inertias 1,2	Defines the various area moments of inertia of the cross section. These defines the settings of the I1, I2, and I12 fields on the PBEAM entry. These values are real values. These properties are optional.
Torsional Constants	Defines the torsional stiffness parameters. This property defines the J fields on the PBEAM entry. This is a list of real values, one for each station location. This property is optional.
Ys of C Points Zs of C Points Ys of D points Zs of D Points Ys of E Points Zs of E Points Ys of F Points Zs of F Points	Defines the Y and Z locations in element coordinates, relative to the shear center for stress data recovery. These define the C1, C2, D1, D2, E1, E2, F1, and F2 fields on the PBEAM entry. These are lists of real values, one for each station location. These properties are optional.
Nonstructural Masses	Defines the mass not included in the mass derived from the material of the element. This is defined in terms of mass per unit length of the beam. This property is the NSM field on the PBEAM entry. This is a list of real values, one for each station location. This property is optional.
NSM Inertia @ Node 1 NSM Inertia @ Node 2	Specified the nonstructural mass moments of inertia per unit length about the nonstructural mass center of gravity at each end of the element. These properties are the NSI(A) and NSI(B) fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
Y of NSM @ Node 1 Z of NSM @ Node 1 Y of NSM @ Node 2 Z of NSM @ Node 2	Defines the offset from the centroid of the cross section to the location of the nonstructural mass. These values are measured in the beam cross-section coordinate system. These are the M1(A), M2(A), M1(B), and M2(B) fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
Shear Stiff, Y Shear Stiff, Z	Defines the shear stiffness values. These properties are the K1 and K2 fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
Shear Relief Y Shear Relief Z	Defines the shear relief coefficients due to taper. These are the S1 and S2 fields on the PBEAM entry. These values can either be real values or references to existing field definitions. These properties are optional.
Warp Coeff. @ Node 1 Warp Coeff. @ Node 2	Specifies the warping coefficient at each end of the element. These properties are the CW(A) and CW(B) fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
Y of NA @ Node 1 Z of NA @ Node 1 Y of NA @ Node 2 Z of NA @ Node 2	Defines the offset from the centroid of the cross section to the location of the neutral axis. These values are measured in the beam cross section coordinate system and are the N1(A), N2(A), N1(B), and N2(B) fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.

General Section Beam (CBEAM)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)
Create	1D	Beam	General Section (CBEAM)

This set of options provides a method of creating beam models with warping due to torsion. The capabilities of this beam properties formulation option are similar to those of the “Tapered Section” formulation, except that warping due to torsion is handled more conveniently.


Note:	Patran will check the element associativity to other elements sharing this property set and will not export user defined pin flags for nodes which are shared by two beams sharing the same node.


Section Name	Specifies a beam section previously created using the beam library
• Value Type	Allows you to define a bar/beam section either by Dimensions (PBARL/PBEAML) or by Properties (PBAR/PBEAM). If Dimensions is choosen, the MSC.Nastran’s built-in section library (Version 69 and later), PBARL/PBEAML, will be used to define the bar/beam. If Properties is chosen, the standard bar/beam properties, PBAR/PBEAM will be used to define the beam section. If the Dimensions Option is set to Dimensions, the Translation Parameters Version must be set to version 69 or later.
Material Name	Defines the material to be used. A list of all materials currently in the database is displayed when data is entered. Either select from the list using the mouse, or type in the name. This defines the setting of the MID field on the PBCOMP entry. This property is required.
Bar Orientation	Defines the local element coordinate system to be used for any cross-sectional properties. This orientation will define the local XY plane, where the x-axis is along the beam. This orientation, after any necessary transformations, defines the value for the X1, X2, X3, or G0 fields on the CBEAM entry. This property is required.
• Value Type	Specifies how the bar orientation is defined: Vector – Specified using a vector Node Id – Specified using an existing node in the beam XY plane When the value type is Vector, it is always input in either the Patran global or some other Patran user defined coordinate system (i.e. <0 1 0 Coord 5>).
• Reference Coordinates	Specifies the MD Nastran coordinate system in which the bar orientation vector will be written to the CBEAM entry: Analysis - Displacement Coordinate System at GA Coord 0 - Basic Coordinate System If Analysis is specified, a G will be written to the first position of the OFFT value on the CBEAM entry. If Coord 0 is specified, a B will be written. Note: The reference coordinate system specified does not affect how the input is interpreted within Patran. Only how it is written to the CBEAM entry.
Offset @ Node 1 Offset @ Node 2	Defines the offset from the nodes to the shear centers of the beam cross section. These orientations are defined as vectors. These properties, after any necessary transformations, become the W1A, W2A, W3A, W1B, W2B, and W3B fields on the CBEAM entry. These properties are optional.
• Value Type	Specifies how the bar orientation is defined: Vector – Specified using a vector This is the only method available. The Reference Coordinate System controls how the vector input is interpreted in Patran.
• Reference Coordinates	Specifies the MD Nastran coordinate system in which the offset vectors will be written to the CBEAM entry and how the vector input will be interpreted in Patran: Analysis - Displacement Coordinate Systems at GA and GB Element - Element Coordinate System If Analysis is specified, a G will be written to the second or third position of the OFFT value on the CBEAM entry. Within Patran, the vector will be interpreted to be in either the Patran global or some other Patran user defined coordinate system (i.e. <0 1 0 Coord 5>). If Element is specified, an E will be written to the second or third position of the OFFT value on the CBEAM entry. Within Patran, the vector will be interpreted to be in the Element coordinate system.
Pinned DOFs @ Node 1 Pinned DOFs @ Node 2	Indicates whether certain degrees of freedom are to be released. By default, all degrees of freedom can transfer forces at the ends of beams. Pin or sliding type connections can be created by releasing specified degrees of freedom. These degrees of freedom are in the element local coordinate system. The values specified here are UX, UY, UZ, RX, RY, RZ, or a combination. These properties define the settings of the PA and PB fields on the CBEAM entry. These properties are optional. Note that if pinned DOF releases are defined within a property set, but the end nodes of the beams are connected to beams of a different property set, then no pinned DOFs will be written for those beams (PA or PB will be left blank). To override this and force the pin flags to be written per the property set, use an "" after the specification for the DOFs. (This may be problematic if the property sets defined different pin DOFs.) For example, if rotation about the 2nd DOF is to be freed, specify "RY." These values must be typed into the data box. Although there is a pull down menu next to the data box showing the valid selections, you will have to type the values in if more than one DOF or the "" is to be specified. Specifying the "" by itself does nothing.
Warping Option	This specifies how contraints should be applied to the warping SPOINTs of unmatched ends within the application region (see continuity rules above). The choices available include “A free B free”, “A fixed B fixed”, “A free B fixed”, “A fixed B free”, or “None”. The choice of “None” is used to disable warping altogether for the current element property set, in which case no SPOINTs will be generated or constrained. Only unmatched ends within the application region will be eligible for constraining, and whether or not a constraint is applied will depend on the option selected, and whether the unmatched end is “End A” or “End B” of its beam element. If no selection is made for this element property, “A free B free” is selected by default.
Warp Coeff. @ Node 1 Warp Coeff. @ Node 2	Specifies the warping coefficient at each end of the element. These properties are the CW(A) and CW(B) fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
Station Distances	Defines stations along each beam element where the section properties will be defined. The values specified here are fractions of the beam length. These values, therefore, are in the range of 0. to 1. These values define the settings of the X/XB fields on the PBEAM record. This field consists of a set of real values separated by legal delimiters, such as white space and/or commas. If this list is entered, then the properties that follow may also be in the form of lists consisting of the same number of values. If they are in the form of a single real value, then that value will apply to all stations of the beam element. This property is optional. If it is not provided, then all other specified section properties apply to the entire beam, and lists of values will not be accepted.
Cross-Sect. Areas	Defines the cross sectional area of the element. This property defines the settings of the A fields on the PBEAM record. This value can be either a real value, a list (if a list of stations has been provided), or a reference to an existing field definition, in which case a single real value will be evaluated for each element of the application region. This property is required.
Inertias 1,1 Inertias 2,2 Inertias 1,2	Defines the various area moments of inertia of the cross section. These values define the settings of the I1, I2, and I12 fields on the PBEAM entry. These values are single real values that apply to the entire beam, or a list of real values if a list of stations has been provided. These properties are optional. If they are not provided, values of 0 will be assumed.
Torsional Constants	Defines the torsional stiffness parameters. This property defines the J fields on the PBEAM entry. This value is a single real value that applies to the entire beam, or a list of real values if a list of stations has been provided. This property is optional. If it is not provided, a value of 0 will be assumed.
Ys of C Points Zs of C Points Ys of D Points Zs of D Points Ys of E Points Zs of E Points Ys of F Points Zs of F Points	Defines the Y and Z locations in element coordinates, relative to the shear center, for stress data recovery. These define the C1, C2, D1, D2, E1, E2, F1, and F2 fields on the PBEAM entry. These values are single real values that apply to the entire beam, or lists of real values if a list of stations has been provided. These properties are optional. If they are not provided, values of 0 will be assumed.
Nonstructural Masses	Defines the mass not included in the mass derived from the material of the element. This is defined in terms of mass per unit length of the beam. This property is the NSM field on the PBEAM entry. This value is a single real value that applies to the entire beam, or a list of real values if a list of stations has been provided. This property is optional. If it is not provided, a value of 0 will be assumed.
NSM Inertia @ Node 1 NSM Inertia @ Node 2	Specifies the nonstructural mass moments of inertia per unit length about the nonstructural mass center of gravity at each end of the element. These properties are the NSI(A) and NSI(B) fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
Y of NSM @ Node 1 Z of NSM @ Node 1 Y of NSM @ Node 2 Z of NSM @ Node 2	Defines the offset from the shear center of the cross section to the location of the nonstructural mass. These values are measured in the beam cross-section coordinate system. These are the M1(A), M2(A), M1(B), and M2(B) fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
Shear Stiff, Y Shear Stiff, Z	Defines the shear stiffness values. These properties are the K1 and K2 fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.
Shear Relief Y Shear Relief Z	Defines the shear relief coefficients due to taper. These are the S1 and S2 fields on the PBEAM entry. These values can either be real values or references to existing field definitions. These properties are optional.
Y of NA @ Node 1 Z of NA @ Node 1 Y of NA @ Node 2 Z of NA @ Node 2	Defines the offset from the shear center of the cross section to the location of the neutral axis. These values are measured in the beam cross-section coordinate system. These are the N1(A), N2(A), N1(B), and N2(B) fields on the PBEAM entry. These values can be either real values or references to existing field definitions. These properties are optional.

Warping due to torsion is enabled by generating MD Nastran SPOINTs to contain the warping degrees of freedom. These SPOINTs are not actually present in the Patran database, and there is no way to recover any results for these SPOINTs. They are created during analysis deck translation, and provide the means to communicate to MD Nastran the continuity and constraint properties of the warping degrees of freedom in the model. These attributes of continuity and constraint are implied in the Patran database through the composition of the element properties application region and the set of options selected. These continuity and constraint attributes apply to both warping SPOINTs and end release flags. This connection of these attributes to the composition of the application region is new in Patran 2001r3, and represents a change in behavior from previous versions of Patran. The general rules of implied continuity are as follows.

1. Within the application region, two beam elements are taken to be continuous if a GRID ID at an end of one of the beam elements matches a GRID ID at one of the ends of the other beam element. If a third beam element in the same application region also contains the same GRID ID, it is assumed that none of the beam elements is continuous at this location. This condition is known as a “multiple junction”. Similarly, if none of the other beam elements in the application region contain a matching GRID ID, the corresponding end of the beam element is taken to be not continuous. This condition is known as an “unmatched end”.

2. If warping is enabled, then all instances of beam element continuity must have the matching GRID ID located at “End A” of one of the beam elements and at “End B” of the other. “End A” and “End B” positions are determined by the order of GRID IDs specified in the element connectivity array, and the positive direction of the x-axis of the element coordinate system points from “End A” to “End B”. If warping is not enabled, this restiction does not apply. If warping is enabled, any violation of this requirement will result in a failure to complete the translation of the finite element model. In this event, the user will have to reverse the direction of the improperly oriented beam elements and initiate the translation again.

3. When warping is enabled, all positions of beam element continuity within an application region will be represented by a single SPOINT at each of these positions, which will be generated at the time of analysis deck translation and will appear on the CBEAM entries for the appropriate end of both of the beam elements that are continuous at each location. If any end release codes have been prescribed for the application region, they will not be applied at locations of beam element continuity. This is new for Patran 2001r3. For earlier versions of Patran, end release codes would be applied to all elements of the application region, regardless of continuity.

4. When warping is enabled, individual SPOINTs are generated for all beam ends that are not continuous. This applies to both “multiple junctions” and “unmatched ends”.

5. The specified end release codes are applied to all discontinuous beam element ends in the application region, whether “multiple junction” or “unmatched end”, with the applied end release codes dependent on what has been prescribed for “End A” and “End B” for the application region. If no end release codes have been prescribed for the application region, none are generated.

6. When warping is enabled, and for unmatched ends only (not multiple junctions), constraints applied to the SPOINTs are specified by the “warping option” specified in the element properties form. For example, if “A free B fixed” has been selected and the unmatched end is “End A” of its beam element, it will not be constrained. If it is “End B” of its element, it will be constrained. The warping SPOINT for a beam element end involved in a multiple junction will not be constrained under any circumstances. If the user wishes to constrain warping for a beam element involved in a multiple junction, he will have to do so by splitting the application region in such a way that the beam element end becomes an “unmatched end” within its new application region.

7. Warping is considered to be enabled when a value has been specified for the warping coefficient at either end of the beam element. When the user selects the “Beam Library” option, values for the warping coefficient get computed autamatically, and thus warping is implicitly enabled. If the user wishes to disable warping while using the Beam Library option, he must choose “None” as his “Warping Option” on the “Input Properties ...” form.

General Section Rod (CROD)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	1D	Rod	General Section Standard	Bar/2

Use this form to create a CROD element and a PROD property. This defines a tension-compression-torsion element of the structural model.

General Section Rod (CONROD)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	1D	Rod	General Section CONROD	Bar/2

Use this form to create a CONROD element. This defines a tension-compression-torsion element of the structural model.

Pipe Section Rod (CTUBE)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	1D	Rod	Pipe Section	Bar/2

Use this form to create a CTUBE element and a PTUBE property. This defines a tension-compression-torsion element with a thin-walled tube cross section.

Scalar Spring (CELAS1/CELAS1D)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	1D	Spring		Bar/2

Use this form to create a CELAS1 or CELAS1D (for SOL 700) element and a PELAS property. This defines a scalar spring of the structural model.

Scalar Damper (CDAMP1/CDAMP1D)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	1D	Damper	Scalar	Bar/2

Use this form to create a CDAMP1 or CDAMP1D (for SOL 700) element and a PDAMP property. This defines a scalar damper element of the structural model.

Viscous Damper (CVISC)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	1D	Damper	Viscous	Bar/2

Use this form to create a CVISC element and a PVISC property. This defines a viscous damper element of the structural model.

Gap (CGAP)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	1D	Gap	Adaptive Nonadaptive	Bar/2

Use this form to create a CGAP element and a PGAP property. This defines a gap or frictional element of the structural model for non-linear analysis.

This is a list of Input Properties available for creating a CGAP element and a PGAP property that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties.


Prop Name	Description
Sliding Stiffness	Defines the artificial shear stiffness of the element when the element is closed. This is the Kt field on the PGAP entry. This property can be either a real value or a reference to an existing field definition. This property is optional.
Static Friction	Defines the static friction coefficient. This property is the MU1 field on the PGAP entry. This value is optional and can be a real scalar or a spatially varying real scalar field.
Kinematic Friction	Defines the kinematic friction coefficient. This property is the MU2 field on the PGAP entry. This value is optional and can be a real scalar or a spatially varying real scalar field.
Max Penetration	Defines the maximum allowable penetration. This property is the TMAX field on the PGAP entry. This value is optional and can be a real scalar or a spatially varying real scalar field.
Max Adjust Ratio	Defines the maximum allowable adjustment ratio. This property is the MAR field on the PGAP entry. This value is optional and can be a real scalar or a spatially varying real scalar field.
Penet. Lower Bound	Defines the lower bound for the allowable penetration. This is the TRMIN field on the PGAP entry. This value is optional and can be a real scalar or a spatially varying real scalar field.
Friction Coeff. y Friction Coeff. Z	Defines the coefficient of friction when sliding occurs along this element in the local y and z directions. These are the MU1 and MU2 fields on the PGAP entry and can be either real values or references to existing field definitions. These properties are optional.

Scalar Mass (CMASS1)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	1D	1D Mass		Bar/2

Use this form to create a CMASS1 element and a PMASS property. This defines a scalar mass element of the structural model.

PLOTEL

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	1D	PLOTEL		Bar/2

Use this form to create a PLOTEL element.

(Scalar) Bush

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	1D	Bush		Bar/2

This is a list of Input Properties available. Use the menu scroll bar on the Input Properties form to view these properties.


Prop Name	Description
Bush Orientation	Element orientation strategy keys off of CID specification. If CID is blank, the element x-axis lies along the line which joins the elements grid points (GA, GB Element Properties/Application Region). The X-Y plane is determined by specifying the Bush Orientation. If a vector input is given, these components define an orientation vectorfrom the first grid point (GA) of the element in the displacement coordinate system at that point (GA). If the Bush Orientation references a grid point ID (Value), this orientation point forms an orientation vector which extends from the first element grid point to the orientation point. If a CID ≥ 0 is specified for Bush Orientation System, the element X,Y, and Z axes are aligned with the coordinate system principal axes. If the CID is for a cylindrical or spherical coordinate system, the first elemental grid point (GA) is used to locate the system. If CID = 0, the elemental coordinate system is the Basic Coordinate System. If no orientation is specified in any form, the element x-axis is along the line which connects the element’s grid points. The material property inputs for this condition must be limited to simple axial and torsional stiffness and damping (k1,k4,B1,B4).
Offset Location	Offset Location (0.0 ≤ s ≤ 1.0) specifies the spring-damper location along the line from GRIDGA to GRIDGB by setting the fraction of the distance from GRIDGA. s=0.50 centers the spring-damper.
Offset Orientation System	Specifies the coordinate system used to locate the spring-damper offset when it is not on the line from GRIDGA to GRIDGB.
Offset Orientation Vector	Provides the location of the spring-damper in space relative to the offset coordinate system. If the offset orientation system is -1 or blank, the offset orientation vector is ignored.
Spring Constant 1 Spring Constant 2 Spring Constant 3 Spring Constant 4 Spring Constant 5 Spring Constant 6 Stiff. Freq Depend 1 Stiff. Freq Depend 2 Stiff. Freq Depend 3 Stiff. Freq Depend 4 Stiff. Freq Depend 5 Stiff. Freq Depend 6	Defines the stiffness associated with a particular degree of freedom. This property is defined in terms of force per unit displacement and can be either a real value or a reference to an existing field definition for defining stiffness vs. frequency.
Stiff. Force/Disp 1 Stiff. Force/Disp 2 Stiff. Force/Disp 3 Stiff. Force/Disp 4 Stiff. Force/Disp 5 Stiff. Force/Disp 6	Defines the nonlinear force/displacement curves for each degree of freedom of the spring-damper system.
Damping Coefficient 1 Damping Coefficient 2 Damping Coefficient 3 Damping Coefficient 4 Damping Coefficient 5 Damping Coefficient 6 Damp. Freq Depend 1 Damp. Freq Depend 2 Damp. Freq Depend 3 Damp. Freq Depend 4 Damp. Freq Depend 5 Damp. Freq Depend 6	Defines the force per velocity damping value for each degree of freedom. This property can be either a real value or a reference to an existing field definition for defining damping vs. frequency
Structural Damping Struc. Damp Freq Depend	Defines the non-dimensional structural damping coefficient (GE1). This property can be either a real value, or a reference to an existing field definition for defining damping vs. frequency.
Stress Recovery Translation Stress Recovery Rotation	Stress Recovery Coefficients. The element stress are computed by multiplying the stress coefficients with the recovered element forces.
Strain Recovery Translation Strain Recovery Rotation	Strain Recovery Coefficients. The element strains are computed by multiplying the strain coefficients with the recovered element strains.

Spot Weld Connector (CWELD)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	1D	Spot Weld Connector		Connector

Note that SPOTWELD properties are created automatically (or pre-existing properties selected) when creating Spotwelds through the Finite Elements application. Therefore no application region is required (or presented) in the element properties application when defining or modifying spotweld properties because the existence of the spotweld itself is the application region for the property set.

Fastener Connector (CFAST)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	1D	Fastener Connector		Connector

Note that FASTENER properties are created automatically (or pre-existing properties selected) when creating Fasteners through the Finite Elements application. Therefore no application region is required (or presented) in the element properties application when defining or modifying fastener properties because the existence of the fastener itself is the application region for the property set.

The formula value can be any of the following:

String
None
Douglas
Huth Hi-Lok in CFRP
Huth Hi-Lok in metal
Huth solid rivet

Note that Douglas or one of several Huth formulations can be used to calculate stiffness values of fastener connections automatically, minimizing the need for manual calculation.

Stiffness coefficients for the CFAST element are calculated in different steps. Generally, either Douglas or three derivatives of Huth formulas are used. Regardless of the selected formula, the axial stiffness is always calculated the same way:

The stiffness is inserted into the KT1 parameter of the PFAST entry. The length of the fastener will be determined by summation of the thickness of the two connected shell elements.

The Douglas formula is*:

The formula according to Huth is*:


	a	b
Hi-Lok in CFRP	0.6667	4.2
Hi-Lok in metal	0.6667	3.0
Solid Rivet	0.4	2.2

In the case of composites, the Douglas and Huth formulas have to be used twice. First, the overall (engineering) Young’s modulus has to be calculated for both directions (E11 and E22), which then has to be applied to the formulas. In this case, the shear stillness of the fastener is direction dependent. For composites or anisotrophic material, the material tensors of the two connected shell elements have to be transformed into the coordinate system of the CFAST element before the Douglas or Huth formula is applied. The resulting stiffness is applied to the KT2 and KT3 parameters on the PFAST entry.

* The following symbols are used in the formulas:


Symbol	Meaning
Ef	Young’s modulus of fastener
df	Diameter of fastener
l	Length of fastener, evaluated from the FE model
E1	Young’s modulus of first property connected to the fastener
t1	Thickness of first property connected to the fastener
E2	Young’s modulus of second property connected to the fastener
t2	Thickness of second property connected to the fastener

Standard Homogeneous Plate (CQUAD4)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	2D	Shell	Homogeneous Standard Formulation	Tri/3, Quad/4 Tri/6, Quad/8

Use this form to create a CQUAD4, CTRIA3, CQUAD8, or CTRIA6 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank to achieve the requested behavior.

This is a list of Input Properties, available for creating a CQUADi and a CTRIAi element and a PSHELL property, that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties.


Prop Name	Description
Plate Offset	Defines the offset of the element’s reference plane from the plane defined by the nodal locations. This is the ZOFFS field on the CQUAD4/8 entry and can be either a real value or a reference to an existing field definition. This property is optional.
Fiber Dist. 1 Fiber Dist. 2	Defines the distance from the element’s reference plane to the bottom and top most extreme fibers, respectively. These properties define the Z1 and Z2 fields on the PSHELL entry and can be either real values or references to existing field definitions. This property is optional.
Nonlinear Formulation	This optional property word can take on any of the three values Automatic, Large Strain, or Small Strain and is only recognized for implicit nonlinear (SOL 400) analyses. Automatic is the default if not specified and determines if large or small strain is appropriate based on the existence of an elastoplastic material constitutive model and/or if the elements are contained in a contact body. If appropriate, the PSHLN1/2 entry is written for this property set. Large Strain forces the PSHLN1/2 entry to be written, regardless; and Small Strain forces it not to be written, regardless. In addition, if large strain is forced or detected, the usage of NLMOPTS, LRGSTRN,0 or 1 is written based on the setting on the Load Increment Parameters form when defining a Subcase. See Static Subcase Parameters for Implicit Nonlinear Solution Type, 369.

Revised Homogeneous Plate (CQUADR)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	2D	Shell	Homogeneous Revised Formulation	Tri/3, Quad/4

Use this form to create a CTRIAR or CQUADR element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank to achieve the requested behavior.

P-Formulation Homogeneous Plate (CQUAD4)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen. Information on this form is used to create input for an adaptive, p-element analysis.


Action	Dimension	Type	Option(s)	Topologies
Create	2D	Shell	Homogeneous P-Formulation	Tri/3, Quad/4,Tri/6, Quad/8, Tri/7, Quad/9, Tri/9, Quad/12, Tri/13, Quad/16

Use this form to create a CQUAD4 or CTRIA3 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior.The p-formulation shell element is supported in MSC.Nastran Version 69 or later. Therefore, the MD Nastran Version in the Translation Parameter form must be set to 69.

This is a list of Input Properties, available for creating a CQUAD4 and a CTRIA3 element, that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties.


Prop Name	Description
Plate Offset	Defines the offset of the element’s reference plane from the plane defined by the nodal locations. This is the ZOFFS field on the CQUAD4 or CTRIA3 entry and can be either a real value or a reference to an existing field definition. This property is optional.
Fiber Dist. 1 Fiber Dist. 2	Defines the distance from the element’s reference plane to the top and bottom most extreme fibers, respectively. These properties define the Z1 and Z2 fields on the PSHELL entry and can be either real values or references to existing field definitions. This property is optional.
Starting P-orders and Maximum P-orders	Polynomial orders for displacement representation within elements. Each contains a list of three integers referring to the directions defined by the P-‑order Coordinate System (default elemental). Starting P-orders apply to the first adaptive cycle. The adaptive analysis process will limit the polynomial orders to the values specified in Maximum P-orders. These are the Polyi fields on the PVAL entry.
P-order Coord. System	The three sets of three integer p-orders above refer to the axes of this coordinate system. By default, this system is elemental. This is the CID field on the PVAL entry.
Activate Error Estimate	Flag that controls whether or not this set of elements participates in the error analysis. This is the ERREST field on the ADAPT entry.
P-order Adaptivity	Controls the particular type of p-order adjustment from adaptive cycle to cycle. This is the TYPE field on the ADAPT entry.
Error Tolerance	The tolerance used to determine if the adaptive analysis is complete. By default this value is equal to 0.1. This is the ERRTOL field on the ADAPT entry.
Stress Threshold Value	Elements with von Mises stress below this value will not participate in the error analysis. By default this value is equal to 0.0. This is the SIGTOL field on the ADAPT entry.
Strain Threshold Value	Elements with von Mises strain below this value will not participate in the error analysis.By default this value is equal to1.0E-8. This is the EPSTOL field on the ADAPT entry.

Standard Laminate Plate (CQUAD4/PCOMP)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	2D	Shell	Laminate Standard Formulation	Tri/3, Quad/4 Tri/6, Quad/8

Use this form to create a CTRIA3, CTRIA6, CQUAD4, or CQUAD8 element and a PCOMP property.


Prop Name	Description
Laminate Options	Laminate option placed on the LAM field of the PCOMP/PCOMPG entry. No option implies all plies must be specified and all stiffness terms developed. MEM - all plies are specified but only membrane terms are computed. BEND - all plies specified but only bending terms computed. SMEAR - all plies specified, stacking sequence ignored and TS/T and 12I/T**3 terms set to zero. SMCORE - all plies specified with the last ply specifying core properties and the previous plies specifying face sheet properties. See the Nastran Quick Reference Guide for more details.
Nonlinear Formulation	This optional property word can take on any of the three values Automatic, Large Strain, or Small Strain and is only recognized for implicit nonlinear (SOL 400) analyses. Automatic is the default if not specified and determines if large or small strain is appropriate based on the existence of an elastoplastic material constitutive model and/or if the elements are contained in a contact body. If appropriate, the PSHLN1/2 entry is written for this property set. Large Strain forces the PSHLN1/2 entry to be written, regardless; and Small Strain forces it not to be written, regardless. In addition, if large strain is forced or detected, the usage of NLMOPTS, LRGSTRN,0 or 1 is written based on the setting on the Load Increment Parameters form when defining a Subcase. See Static Subcase Parameters for Implicit Nonlinear Solution Type, 369.


Note:	TREF is written to PCOMP from the value defined on the first MAT8 entry defined in the composite, or in other words, from the material of the first ply in the layup. The value of GE is written to PCOMP as the sum of all GE values on all plies, scaled based on the percentage thickness of each ply. To get values for TREF and GE from the PCOMP entry, the 2D/Shell/Thin/Laminate/Standard and Revised formulations need to have property words used to define these values. If the values are not defined then the values are retrieved from the MAT8 material card.

Revised Laminate Plate (CQUADR/PCOMP)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	2D	Shell	Laminate Revised Formulation	Tri/3, Quad/4

Use this form to create a CQUADR or CTRIAR element and a PCOMP property.


Note:	TREF is written to PCOMP from the value defined on the first MAT8 entry defined in the composite, or in other words, from the material of the first ply in the layup. The value of GE is written to PCOMP as the sum of all GE values on all plies, scaled based on the percentage thickness of each ply. To get values for TREF and GE from the PCOMP entry, the 2D/Shell/Thin/Laminate/Standard and Revised formulations need to have property words used to define these values. If the values are not defined then the values are retrieved from the MAT8 material card.

Standard Equivalent Section Plate (CQUAD4)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	2D	Shell	Equivalent Section Standard Formulation	Tri/3, Quad/4 Tri/6, Quad/8

This is a list of Input Properties available for creating a CTRIA3, CTRIA6, CQUAD4, or CQUAD8 element and a PSHELL property that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties.


Prop Name	Description
Bending Stiffness	Defines the bending stiffness parameter. This is the 12I/T3 field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Thickness Ratio	Defines the ratio of transverse shear thickness to the membrane thickness. This property is the TS/T field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Nonstructural Mass	Defines mass not included in the mass derived from the material of the element. This is defined in terms of mass per unit area of the element. This property is the NSM field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Plate Offset	Defines the offset of the element’s reference plane from the plane defined by the nodal locations. This property is the ZOFFS field on the CTRIA3, CTRIA6, CQUAD4, or CQUAD8 entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Fiber Distance 1 Fiber Distance 2	Defines the distance from the element’s reference plane to the top and bottom most extreme fibers, respectively. These properties are the Z1 and Z2 fields on the PSHELL entry. These values can be either real values or references to existing field definitions. These properties are optional.
Nonlinear Formulation	This optional property word can take on any of the three values Automatic, Large Strain, or Small Strain and is only recognized for implicit nonlinear (SOL 400) analyses. Automatic is the default if not specified and determines if large or small strain is appropriate based on the existence of an elastoplastic material constitutive model and/or if the elements are contained in a contact body. If appropriate, the PSHLN1/2 entry is written for this property set. Large Strain forces the PSHLN1/2 entry to be written, regardless; and Small Strain forces it not to be written, regardless. In addition, if large strain is forced or detected, the usage of NLMOPTS, LRGSTRN,0 or 1 is written based on the setting on the Load Increment Parameters form when defining a Subcase. See Static Subcase Parameters for Implicit Nonlinear Solution Type, 369.

Revised Equivalent Section Plate (CQUADR)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	2D	Shell	Equivalent Section Revised Formulation	Tri/3, Quad/4

Use this form to create a CTRIAR or CQUADR element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior.

This is a list of Input Properties available for creating a CTRIAR or CQUADR element and a PSHELL property that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties.


Prop Name	Description
Bending Stiffness	Defines the bending stiffness parameter. This property is the 12I/T3 field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Thickness Ratio	Defines the ratio of transverse shear thickness to the membrane thickness. This is the TS/T field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Nonstructural Mass	Defines mass not included in the mass derived from the material of the element. This property is defined in terms of mass per unit area of the element. This is the NSM field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Fiber Distance 1 Fiber Distance 2	Defines the distance from the element’s reference plane to the top and bottom most extreme fibers respectively. These properties are the Z1 and Z2 fields on the PSHELL entry. These values can be either real values or references to existing field definitions. These properties are optional.
Nonlinear Formulation	This optional property word can take on any of the three values Automatic, Large Strain, or Small Strain and is only recognized for implicit nonlinear (SOL 400) analyses. Automatic is the default if not specified and determines if large or small strain is appropriate based on the existence of an elastoplastic material constitutive model and/or if the elements are contained in a contact body. If appropriate, the PSHLN1/2 entry is written for this property set. Large Strain forces the PSHLN1/2 entry to be written, regardless; and Small Strain forces it not to be written, regardless. In addition, if large strain is forced or detected, the usage of NLMOPTS, LRGSTRN,0 or 1 is written based on the setting on the Load Increment Parameters form when defining a Subcase. See Static Subcase Parameters for Implicit Nonlinear Solution Type, 369.

P-Formulation Equivalent Section Plate (CQUAD4)


Action	Dimension	Type	Option(s)	Topologies
Create	2D	Shell	Equivalent Section P-Formulation	Tri/3, Quad/4, Tri/6, Quad/8, Tri/7, Quad/9, Tri/9, Quad/12, Tri/13, Quad/16

Use this form to create a CQUAD4, or CTRIA3 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior. The p-formulation shell element is supported in MSC.Nastran Version 69 or later. Therefore, the MSC.Nastran Version in the Translation Parameter form must be set to 69.

This is a list of Input Properties, available for creating a CQUAD4 and a CTRIA3 element that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties.


Prop Name	Description
Bending Stiffness	Defines the bending stiffness parameter. This property is the 12I/T3 field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Thickness Ratio	Defines the ratio of transverse shear thickness to the membrane thickness. This is the TS/T field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Nonstructural Mass	Defines mass not included in the mass derived from the material of the element. This property is defined in terms of mass per unit area of the element. This is the NSM field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Plate Offset	Defines the offset of the element’s reference plane from the plane defined by the nodal locations. This is the ZOFFS field on the CQUAD4 or CTRIA3entry and can be either real value or reference to an existing field definition. This property is optional.
Fiber Dist. 1 Fiber Dist. 2	Defines the distance from the element’s reference plane to the top and bottom most extreme fibers, respectively. These properties define the Z1 and Z2 fields on the PSHELL entry and can be either real value or references to existing field definitions. This property is optional.
Starting P-orders and Maximum P-orders	Polynomial orders for displacement representation within elements. Each contains a list of three integers referring to the directions defined by the P-order Coordinate System (default elemental). Starting P-orders apply to the first adaptive cycle. The adaptive analysis process will limit the polynomial orders to the values specified in Maximum P-orders. These are the Polyi fields in the PVAL entry.
P-order Coord. System	The three sets of three integer p-orders above refer to the axes of this coordinate system. By default, this system is elemental. This is the CID field on the PVAL entry.
Activate Error Estimate	Flag controlling whether this set of elements participates in the error analysis. This is the ERREST field in the ADAPT entry.
P-order Adaptivity	Controls the particular type of p-order adjustment from adaptive cycle to cycle. This is the TYPE field on the ADAPT entry.
Error Tolerance	The tolerance used to determine if the adaptive analysis is complete. By default, equal to 0.1. This is the ERRTOL field on the ADAPT entry.
Stress Threshold Value	Elements with von Mises stress below this value will not participate in the error analysis. By default, equal to 0.0. This is the SIGTOL field on the ADAPT entry.
Strain Threshold Value	Elements with von Mises strain below this value will not participate in the error analysis. By default, equal to1.0E-8. This is the EPSTOL field on the ADAPT entry.

Field Point Mesh (CQUAD4/TRIA3)(Exterior Acoustics)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	2D	Shell	Field Point Mesh	Tri/3, Quad/4

Use this form to create a CTRIA3, CQUAD4 elements for creating acoustic field point mesh for an exterior acoustics analysis. No property cards are created. The material referenced should be the same as that defined for the 3D solid elements and exterior acoustic infinite elements used to define the surrounding fluid environment of the structure, although no actual materials is written. In order to recover results on these meshes, you must set the output request ACFPFRESULT.

Each acoustic field point mesh defined is written to a seperate section of the bulk data using the BEGIN AFPM=id.

Standard Bending Panel (CQUAD4)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	2D	Bending Panel	Standard Formulation	Tri/3, Quad/4 Tri/6, Quad/8

This is a list of Input Properties available for creating a CTRIA3, CTRIA6, CQUAD4 or CQUAD8 element and a PSHELL property that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties.


Prop Name	Description
Fiber Dist. 1 Fiber Dist. 2	Defines the distance from the element’s reference plane to the top and bottom most extreme fibers respectively. These properties define the Z1 and Z2 fields on the PSHELL entry and these values can be either real values or references to existing field definitions. These properties are optional.

Revised Bending Panel (CQUADR)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	2D	Bending Panel	Revised Formulation	Tri/3, Quad/4

Use this form to create a CTRIAR or CQUADR element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior.

P-Formulation Bending Panel (CQUAD4)


Action	Dimension	Type	Option(s)	Topologies
Create	2D	Bending Panel	P- Formulation	Tri/3, Quad/4, Tri/6, Quad/8, Tri/7, Quad/9, Tri/9, Quad/12, Tri/13, Quad/16

Use this form to create a CTRIA3, or CQUAD4 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior. The p-formulation shell element is supported in MSC.Nastran Version 69 or later. Therefore, the MSC.Nastran Version in the Translation Parameters form must be set to 69.

This is a list of Input Properties available for creating a CTRIA3 or CQUAD4 element and a PSHELL property that were not shown on the previous page. Use the menu scroll bar on the Input Properties form to view these properties.


Prop Name	Description
Nonstructural Mass	Defines mass not included in the mass derived from the material of the element. This property is defined in terms of mass per unit area of the element. This is the NSM field on the PSHELL entry. This value can be either a real value or a reference to an existing field definition. This property is optional.
Fiber Dist. 1 Fiber Dist. 2	Defines the distance from the element’s reference plane to the top and bottom most extreme fibers, respectively. These properties define the Z1 and Z2 fields on the PSHELL entry. These values can be either real values or references to existing field definitions. These properties are optional.
Starting P-orders and Maximum P-orders	Polynomial orders for displacement representation within elements. Each contains a list of three integers referring to the directions defined by the P-order Coordinate System (default elemental). Starting P-orders apply to the first adaptive cycle. The adaptive analysis process will limit the polynomial orders to the values specified in Maximum P-orders. These are the Polyi fields on the PVAL entry.
P-order Coord. System	The three sets of three integer p-orders above refer to the axes of this coordinate system. By default this system is elemental. This is the CID field on the PVAL entry.
Activate Error Estimate	Flag controlling whether this set of elements participates in the error analysis. This is the ERREST field on the ADAPT entry.
P-order Adaptivity	Controls the particular type of p-order adjustment from adaptive cycle to cycle. This is the TYPE field on the ADAPT entry.
Error Tolerance	The tolerance used to determine if the adaptive analysis is complete. By default this value is equal to 0.1. This is the ERRTOL field on the ADAPT entry.
Stress Threshold Value	Elements with von Mises stress below this value will not participate in the error analysis. By default this value is equal to 0.0. This is the SIGTOL field on the ADAPT entry.
Strain Threshold Value	Elements with von Mises strain below this value will not participate in the error analysis. By default this value is equal to1.0E-8. This is the EPSTOL field on the ADAPT entry.

Standard Axisymmetric Solid (CQUADX,CTRIAX/X6)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	2D	2D Solid	Axisymmetric	Tri/3, Tri/6

Use this form to create a CTRIAX6 axisymmetric solid element for non SOL 400 runs. This defines an isoparametric and axisymmetric triangular cross section ring element with midside nodes for non SOL 400 runs. For SOL 400 runs, CQUADX and/or CTRIAX entries and a PLPLANE and PSHLN2 entry are written instead based on the setting of the Nonlinear Formulation. If left blank or set to automatic, a PSHLN2 is written only if the property set contains deformable contact bodies or plasticity is defined. To force a PSHLN2 to write, set the Nonlinear Formulation to Large Strain. To force a PSHLN2 to be excluded (not written), set the Nonlinear Formulation to Small Strain.

PLPLANE Axisymmetric Solid (CTRIAX, CQUADX)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option 1	Option 2	Topologies
Create	2D	2D Solid	Axisymmetric	Hyperelastic PLPLANE	Tri/3, Tri/6, QUAD/4, QUAD/8

Use this form to create axisymmetric solid elements. This defines an isoparametric and axisymmetric cross section ring element with or without midside nodes.

2D Axi-Symmetric Laminated Solid Composite

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	2D	2D Solid	Laminate	CQUADX

Use this form to create CQUADX elements and a PLCOMP property.

The DIRECT field of these cards is negative for the "Total" option where ply thicknesses are the actual thicknesses and positive for the "Total - %thicknesses" option where ply thicknesses are defined as percentages of the total ply stack thickness.

Standard Plane Strain Solid (CQUAD4)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	2D	2D Solid	Plane Strain Standard Formulation	Tri/3, Quad/4 Tri/6, Quad/8

Use this form to create a CTRIA3, CTRIA6, CQUAD4, or CQUAD8 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested plane strain behavior for non SOL 400 runs. For SOL 400 runs a PLPLANE and PSHLN2 entry are written instead based on the setting of the Nonlinear Formulation. If left blank or set to automatic, a PSHLN2 is written only if the property set contains deformable contact bodies or plasticity is defined. To force a PSHLN2 to write, set the Nonlinear Formulation to Large Strain. To force a PSHLN2 to be excluded (not written), set the Nonlinear Formulation to Small Strain.

Revised Plane Strain Solid (CQUADR)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	2D	2D Solid	Plane Strain Revised Formulation	Tri/3, Quad/4

Use this form to create a CTRIAR or CQUADR element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior.

P-Formulation Plane Strain Solid (CQUAD4)


Action	Dimension	Type	Option(s)	Topologies
Create	2D	2D Solid	Plane Strain P- Formulation	Tri/3, Quad/4, Tri/6, Quad/8, Tri/7, Quad/9, Tri/9, Quad/12, Tri/13, Quad/16

Use this form to create a CQUAD4 or CTRIA3 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior. The p-formulation shell element is supported in MSC.Nastran Version 69 or later. Therefore, the MSC.Nastran Version in the Translation Parameters form must be set to 69.

Additional properties on the form which do not appear on the previous page are:


Prop Name	Description
P-order Coord. System	The three sets of three integer p-orders above refer to the axes of this coordinate system. By default, this system is elemental. This is the CID field on the PVAL entry.
Activate Error Estimate	Flag controlling whether this set of elements participates in the error analysis. This is the ERREST field on the ADAPT entry.
P-order Adaptivity	Controls the particular type of p-order adjustment from adaptive cycle to cycle. This is the TYPE field on the ADAPT entry.
Error Tolerance	The tolerance used to determine if the adaptive analysis is complete. By default this value is equal to 0.1. This is the ERRTOL field on the ADAPT entry.
Stress Threshold Value	Elements with von Mises stress below this value will not participate in the error analysis. By default this value is equal to 0.0. This is the SIGTOL field on the ADAPT entry.
Strain Threshold Value	Elements with von Mises strain below this value will not participate in the error analysis. By default this value is equal to 1.0E-8. This is the EPSTOL field on the ADAPT entry.

Plane Stress (CTRIA3/6,CQUAD4/8)


Action	Dimension	Type	Option(s)	Topologies
Create/Modify	2D	2D Solid		Tri/6, Quad/4, Quad/8

This element is meant for use with SOL 400 only (MD Nastran 2010 or greater). Use this form to create a CTRIA6 (CTRIA3 not supported by MD Nastran), CQUAD4/8 element and a PLPLANE plus PSHLN2 entries are based on the setting of the Nonlinear Formulation. If left blank or set to automatic, a PSHLN2 is written only if the property set contains deformable contact bodies or plasticity is defined. To force a PSHLN2 to write, set the Nonlinear Formulation to Large Strain. To force a PSHLN2 to be excluded (not written), set the Nonlinear Formulation to Small Strain.

Other inputs are similar to Plane Strain Standard Formulation except that a thickness must be specified.

Infinite (Exterior Acoustic Element)(CACINF3/CACINF4)

These elements are used in exterior acoustic analysis (frequency response) and placed on the outside of the solid mesh representing the fluid (coincident with the outside surface). The must share the same nodes as the solid mesh. They simulate the fluid proprties reaching to infinity beyond the boundary of the solid mesh representing the fluid. The surfaces that these elements connect to must be convex. However it is not necessary that the surface be smooth. They also take on the same fluid proprties as the solid fluid mesh.


Action	Dimension	Type	Option(s)	Topologies
Create	2D	2D Solid	Infinite	Tri/3, Quad/4

Use this form to create a CACINF3, CACINF4 elements and a PACINF property. The appropriate fields on the PACINF entry are filled in or left blank in order to achieve the requested behavior.

2D Plane Strain Laminated Solid Composite

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	2D	2D Solid	Laminate	QUAD/4, QUAD/8

Use this form to create quadratic elements and a PLCOMP property.

Standard Membrane (CQUAD4)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	2D	Membrane	Standard Formulation	Tri/3, Quad/4 Tri /6, Quad/8

Revised Membrane (CQUADR)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	2D	Membrane	Revised Formulation	Tri/3, Quad/4

Use this form to create a CTRIAR or CQUADR element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior.

P-Formulation Membrane (CQUAD4)


Action	Dimension	Type	Option(s)	Topologies
Create	2D	Membrane	P- Formulation	Tri/3, Quad/4, Tri/6, Quad/8, Tri/7, Quad/9. Tri/9, Quad/12, Tri/13, Quad/16

Use this form to create a CQUAD4 or CTRIA3 element and a PSHELL property. The appropriate fields on the PSHELL entry are filled in or left blank in order to achieve the requested behavior. The p-formulation shell element is supported in MSC.Nastran Version 69 or later. Therefore, the MSC.Nastran Version in the Translation Parameters form must be set to 69.

Additional properties on the form which do not appear on the previous page are:


Prop Name	Description
P-order Coord. System	The three sets of three integer p-orders above refer to the axes of this coordinate system. By default this system is elemental. This is the CID field on the PVAL entry.
Activate Error Estimate	Flag controlling whether this set of elements participates in the error analysis. This is the ERREST field on the ADAPT entry.
P-order Adaptivity	Controls the particular type of p-order adjustment from adaptive cycle to cycle. This is the TYPE field on the ADAPT entry.
Error Tolerance	The tolerance used to determine if the adaptive analysis is complete. By default this value is equal to 0.1. This is the ERRTOL field on the ADAPT entry.
Stress Threshold Value	Elements with von Mises stress below this value will not participate in the error analysis. By default this value is equal to 0.0. This is the SIGTOL field on the ADAPT entry.
Strain Threshold Value	Elements with von Mises strain below this value will not participate in the error analysis. By default this value is equal to 1.0E-8. This is the EPSTOL field on the ADAPT entry.

Shear Panel (CSHEAR)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	2D	Shear Panel		Quad/4

Use this form to create a CSHEAR element and a PSHEAR property. This defines a shear panel element of the structural model.

Additional properties on the form which do not appear on the previous page are:


Nonlinear Formulation	This optional property word can take on any of the three values Automatic, Large Strain, or Small Strain and is only recognized for implicit nonlinear (SOL 400) analyses. Automatic is the default if not specified and determines if large or small strain is appropriate based on the existence of an elastoplastic material constitutive model and/or if the elements are contained in a contact body. If appropriate, the PSHEARN entry is written for this property set. Large Strain forces the PSHEARN entry to be written, regardless; and Small Strain forces it not to be written, regardless. In addition, if large strain is forced or detected, the usage of NLMOPTS, LRGSTRN,0 or 1 is written based on the setting on the Load Increment Parameters form when defining a Subcase. See Static Subcase Parameters for Implicit Nonlinear Solution Type, 369.

Solid (CHEXA)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option 1	Option 2	Topologies
Create/ Modify	3D	Solid	Homogeneous	Standard Formulation Solid Shell	Tet4/10, Wedge6/15 Hex8/20

Use this form to create a CHEXA, CTETRA, or CPENTA element and a PSOLID property for Standard Formulations. A Solid Shell definition is identical to a Standard Formulation in that it also creates the elements plus a PSOLID property, but is meant for use in SOL 400 only and creates the additional PSLDN1 entry (the nonlinear formulation property does not need to be defined and is not included on the Input Properties form).

Additional properties on the form which do not appear on the previous page are:


Nonlinear Formulation	This optional property word can take on any of the three values Automatic, Large Strain, or Small Strain and is only recognized for implicit nonlinear (SOL 400) analyses. Automatic is the default if not specified and determines if large or small strain is appropriate based on the existence of an elastoplastic material constitutive model and/or if the elements are contained in a contact body. If appropriate, the PSLDN1 entry is written for this property set. Large Strain forces the PSLDN1 entry to be written, regardless; and Small Strain forces it not to be written, regardless. In addition, if large strain is forced or detected, the usage of NLMOPTS, LRGSTRN,0 or 1 is written based on the setting on the Load Increment Parameters form when defining a Subcase. See Static Subcase Parameters for Implicit Nonlinear Solution Type, 369.

P-Formulation Solid (CHEXA)


Action	Dimension	Type	Option(s)	Topologies
Create	3D	Solid	P-Formulation	Tet/4, Wedge/6 Hex/8, Tet/10 Wedge/15, Hex/20, Tet/16, Tet/40, Wedge/24,Wedge/52, Hex/32, Hex/64

Use this form to create a CHEXA, CTETRA, or CPENTA element and a PSOLID property.

Additional properties on the form which do not appear on the previous page are:


Prop Name	Description
P-order Coord. System	The three sets of three integer p-orders above refer to the axes of this coordinate system. By default, this system is elemental. This is the CID field on the PVAL entry.
Activate Error Estimate	Flag controlling whether this set of elements participates in the error analysis. This is the ERREST field on the ADAPT entry.
P-order Adaptivity	Controls the particular type of p-order adjustment from adaptive cycle to cycle. This is the TYPE field on the ADAPT entry.
Error Tolerance	The tolerance used to determine if the adaptive analysis is complete. By default the value is equal to 0.1. This is the ERRTOL field on the ADAPT entry.
Stress Threshold Value	Elements with von Mises stress below this value will not participate in the error analysis. By default the value is equal to 0.0. This is the SIGTOL field on the ADAPT entry.
Strain Threshold Value	Elements with von Mises strain below this value will not participate in the error analysis. By default the value is equal to 1.0E-8. This is the EPSTOL field on the ADAPT entry.
Integration Network	Defines the type of integration network to be used. This property is the IN field on the PSOLID entry and can be set to Bubble, Two, or Three. This property is optional.
Integration Scheme	Defines where the output for these elements are to be reported. This can be set to either Gauss or Grid. This property is the STRESS field on the PSOLID entry. This property is optional.

Hyperelastic Plane Strain Solid (CQUAD4)


Action	Dimension	Type	Option(s)	Topologies
Create	2D	2D Solid	Plane Strain Hyperelastic Formulation	Tri/3, Quad/4, Tri/6, Quad/8, Quad/9

Use this form to create a CQUAD, CQUAD4, CQUAD8, CTRIA3, or CTRIA6 element and a PLPLANE property.

Hyperelastic Axisym Solid (CTRIAX6)


Action	Dimension	Type	Option(s)	Topologies
Create	2D	2D Solid	Axisymmetric Hyperelastic Formulation	CQUADX, CTRIAX

Use this form to create a CQUADX or CTRIAX element and a PLPLANE property.

Hyperelastic Solid (CHEXA)


Action	Dimension	Type	Option(s)	Topologies
Create	3D	Solid	Hyperelastic Formulation	HEX, PENT, TET

Use this form to create a CHEXA, CTETRA, or CPENTA element and a PLSOLID property.

Additional properties on the form which do not appear on the form above:


Nonlinear Formulation	This optional property word can take on any of the three values Automatic, Large Strain, or Small Strain and is only recognized for implicit nonlinear (SOL 400) analyses. Automatic is the default if not specified and determines if large or small strain is appropriate based on the existence of an elastoplastic material constitutive model and/or if the elements are contained in a contact body. If appropriate, the PSLDN1 entry is written for this property set. Large Strain forces the PSLDN1 entry to be written, regardless; and Small Strain forces it not to be written, regardless. In addition, if large strain is forced or detected, the usage of NLMOPTS, LRGSTRN,0 or 1 is written based on the setting on the Load Increment Parameters form when defining a Subcase. See Static Subcase Parameters for Implicit Nonlinear Solution Type, 369.

3D Laminate Solid (CHEXA)

This subordinate form appears when the Input Properties button is selected on the Element Properties form and the following options are chosen.


Action	Dimension	Type	Option(s)	Topologies
Create	3D	Solid	Laminate	HEX, PENT, TET

Use this form to create CHEXA elements and a PCOMP (SOL 600) or PCOMPLS (SOL400) property. For Property 3D Solid / Laminate you can now define the Integration Scheme. Note that only Assumed Strain is allowed for HEX8 elements only when ply stack direction is in Z-element diretion and the ply thicknesses have been defined as percent thicknesses. Any other combination will revert the integration scheme to the Nastran default for linear or quadratic elements.