NASTRAN

Autodesk Simulation Mechanical will export models in the MSC Nastran format using the Export Third-Party FEA command. The program will also import MSC Nastran models using the Open dialog box.

Alternatively, you can export Simulation Mechanical models directly to the Autodesk Nastran Editor, in which case the model translation follows NEi / Autodesk Nastran conventions. For more information on this alternative Nastran model output capability, see the Export a Model to the Autodesk Nastran Editor page.

In addition, you can Merge the results of a Nastran Editor simulation back into the original Simulation Mechanical model, which was the source of the Nastran Editor model. See the Display Nastran Editor Results in Simulation Mechanical page for more information.

The tables on this page list the element types, material models, loads, constraints, and the corresponding Nastran card used for each. The information is applicable to both Nastran translation workflows—Third-Party FEA (Nastran) and the Autodesk Nastran Editor.

Static stress with linear material models:

The following table explains how each NASTRAN item is handled when it is transferred. This table can be reversed for information on how Simulation Mechanical items are translated to the NASTRAN input file with the exceptions listed below the table.

	NASTRAN	Autodesk Simulation Mechanical
Truss Elements	PROD / CROD or CONROD	Linear truss
Beam Elements	PBAR / CBAR	Linear beam (offsets and end releases will also be transferred from CBAR)
	PBEAM / CBEAM	Linear beam with constant cross-sectional properties (the first set of cross-sectional properties will be used)
	PLOAD1	Linear beam distributed loads
Gap Elements	PGAP / CGAP	Gap element
Plate Elements	PSHELL / CQUAD4 / CQUADR / CTRIA3 / CTRIAR with values in the MID1 and MID2 fields	Linear plate (material properties will depend on the MAT type as described below)
	PSHELL / CQUAD8 / CTRIA6 with values in the MID1 and MID2 fields	Linear plate (midside nodes will not be translated)
	MAT1	Isotropic material model
	MAT2	If the material is orthotropic material model, an orthotropic material model will be used; if the material is anisotropic, no material properties will be translated
	MAT8	Orthotropic material model
	PLOAD4	Normal pressure or traction (the orientation for the first element will be used to orient the pressure on the entire part)
Membrane Elements	PSHELL / CQUAD4 / CQUADR / CTRIA3 / CTRIAR with a value in only the MID1 field	Linear membrane (material properties will depend on the MAT type as described below)
	PSHELL / CQUAD8 / CTRIA6 with a value in only the MID1 field	Linear membrane (midside nodes will not be translated)
	MAT1	Isotropic material model
	MAT2	If the material is orthotropic material model, an orthotropic material model will be used; if the material is anisotropic, no material properties will be translated
	MAT8	Orthotropic material model
	PLOAD4	Normal pressure
Thin Composites	PSHELL / CQUAD4 / CQUADR / CTRIA3 / CTRIAR	Linear thin composite (only material properties from a MAT8 card with orthogonal material axes will be translated, and midside nodes will not be translated)
	PLOAD4	Normal pressure
Brick (hybrid mesh) and Tetrahedral Elements	PSOLID / CHEXA / CPENTA / CPYRAM (or CPYRA)1 / CTETRA	Linear bricks and tetrahedra (Material properties will depend on the MAT type as described below. If all the midside nodes are present, they will be translated. If one of the midside nodes are not present, no midside nodes will be translated.)
	MAT1	Isotropic material model
	MAT9	If the material is orthotropic material model, an orthotropic material model will be used; if the material is anisotropic, no material properties will be translated
	MATT1	Temperature dependent isotropic
	MATT9	If the material is orthotropic material model, an orthotropic material model will be used; if the material is anisotropic, no material properties will be translated
	PLOAD4	Normal pressure
Rigid Elements	RBE2	Rigid element
Other Element Types	PSHEAR / CSHEAR	The CSHEAR element and properties are imported as if they are PSHELL and CQUAD4 cards.
Contact	CONTACTGENERATE	Defines the default contact type and options. For bonded/welded contact with matched meshes, this card is not used. Instead nodes are merged where parts meet to establish the connection.
	BSCONP	Specifies the contact type (PTYPE) and options (such as friction) for explicitly defined contact pairs.
	BSSEG	Defines the two surface face segments
	PTYPE 1 through PTYPE 10	Penetration type. The value of this parameter represents the following contact types: 1: Unsymmetric general contact 2: Symmetric general contact 3: Unsymmetric welded contact 4: Symmetric welded contact 5: Unsymmetric bidirectional sliding contact 6: Symmetric bidirectional sliding contact 7: Unsymmetric rough contact 8: Symmetric rough contact 9: Unsymmetric offset welded contact 10: Symmetric offset welded contact
	MPC	Multipoint constraints (for smart bonded contact).
Nodal Loads and Constraints	FORCE	Nodal force
	MOMENT	Nodal moment
	SPC	If there is a displacement magnitude, this will translate as a nodal displacement boundary element, otherwise this will translate as a nodal boundary condition
	SPC1	Nodal boundary condition
	SPCD	Nodal displacement boundary element
	CELAS2	Spring element
	TEMP	Nodal temperature
Body Loads	GRAV	Acceleration/gravity
	RFORCE	Centrifugal force
	TEMPD	Default nodal temperature

Result Types Supported: Simulation Mechanical can translate the results to and from the NASTRAN OP2 file.

The following results will be translated from the NASTRAN file.

• Nodal displacements
• Element forces and moments
• Force in gap elements
• Element stress
• Element strain

The following results will be translated to the NASTRAN file.

• Nodal displacements
• Element forces and moment
• Element stress
• Element strain
• Composite results

Natural Frequency and Critical Buckling Load

The following table explains how each NASTRAN item is handled when it is transferred. This table can be reversed for information on how Simulation Mechanical items are translated to the NASTRAN input file with the exceptions listed below the table.

NASTRAN	Simulation Mechanical
EIGRL, EIGR	Number of frequencies or buckling modes to be solved

Result Types Supported: Simulation Mechanical can translate the results to and from the NASTRAN OP2 file.

The following results will be translated from the NASTRAN file.

• Natural frequencies
• Mode shapes
• Buckling multipliers

Static Stress with Nonlinear Material Models

Nonlinear analyses support both linear and nonlinear material models. Refer to the Static Stress with Linear Material Models section above for the supported linear element and material types, supported loads and constraints, corresponding Nastran cards, and translated results. One terminology exception: in nonlinear analyses, Simulation Mechanical employs Shell elements rather than Plates.

The following table lists the additional nonlinear elements, material models, and solution parameters that are supported for nonlinear Nastran models. This information is applicable to models solved within Simulation Mechanical using a Nastran processor, models exported to the Autodesk Nastran Editor, and models exported to a Nastran deck (Export Third-Party FEA).

	NASTRAN	Autodesk Simulation Mechanical
Brick (hybrid mesh) and Tetrahedral Elements	PSOLID / CHEXA / CPENTA / CPYRAM (or CPYRA)1 / CTETRA	Nonlinear bricks and tetrahedra (available nonlinear material models as listed below)
	MAT1, MAT4, and MATS1	von Mises with Isotropic Hardening material model
	MAT1, MAT4, and MATS1	von Mises with Kinematic Hardening material model
Beam Elements	CBAR / PBAR	Nonlinear beams (available linear and nonlinear material models as listed below)
	MAT1 and MAT4	Isotropic material model
	MAT1, MAT4, and MATS1	von Mises with Isotropic Hardening material model
	MAT1, MAT4, MATT1, and TABLEM1	Temperature Dependent Isotropic material model
Contact	PTYPE 1 through PTYPE 4 PTYPE 9 / PTYPE 10	Penetration type. The value of this parameter represents the following contact types. (This list includes all contact types supported for nonlinear static stress analyses): 1: Unsymmetric general contact 2: Symmetric general contact 3: Unsymmetric welded contact 4: Symmetric welded contact 9: Unsymmetric offset welded contact 10: Symmetric offset welded contact
Nonlinear Solution Parameters	PARAM
	CONTACTSTAB	Surface contact solution stabilization option
	INTOUT	Intermediate results output request
	LGDISP	Controls the use of large displacement and follower force effects and differential stiffness.
	NINC	Number of increments
	NLAYERS	Specifies the number of nonlinear material layers in quad and tri elements
	NLCOMPPLYFAIL	Nonlinear composite Progressive Ply Failure Analysis (PPFA) option
	NLINDATABASE	Controls the storage and retrieval of nonlinear data (such as loads, displacements, stress, and strain).
	NLTOQUAD	Controls tension-only quad element support
	SLINEKSFACT	Specifies the initial penalty values used in slide line and surface contact analyses.
	SLINEMAXPENDIST	Specifies the maximum slide line and surface contact element penetration distance.
	SLINEMAXACTDIST	Specifies the maximum slide line and surface contact element activation distance.
	SLINEOFFSETTOL	Specifies the tolerance for automatically converting surface weld elements to offset weld elements.
	SLINESLIDETYPE	Contact penalty stiffness update method.
	SLINESTABKSFACT	Used to stabilize surface contact in nonlinear static solutions (adds normal and in-plane stabilization stiffness).

Steady-state heat transfer

The following table explains how each NASTRAN item is handled when it is transferred. This table can be reversed for information on how Simulation Mechanical items are translated to the NASTRAN input file with the exceptions listed below the table.

	NASTRAN	Autodesk Simulation Mechanical
Rod Elements	PROD / CROD or CONROD	Thermal rod
	MAT4	Isotropic material model
	MATT4	Isotropic temperature-dependent material model
Plate Elements	PSHELL / CQUAD4 / CQUADR / CTRIA3 / CTRIAR	Thermal plate (material properties will depend on the MAT type as described below)
	MAT4	Isotropic material model
	MATT4	Temperature-dependent isotropic material model
	MAT5	Orthotropic material model
	MATT5	Temperature-dependent orthotropic material model
Brick (hybrid mesh) and Tetrahedral Elements	PSOLID / CHEXA / CPENTA / CPYRAM (or CPYRA)1 / CTETRA	Thermal brick (material properties will depend on the MAT type as described below)
	MAT4	Isotropic material model
	MAT5	Orthotropic material model
	MATT5	Temperature-dependent orthotropic
Thermal Loads	QBDY1	Thermal heat flux
	CHBDYG / RADBC / RADM	Radiation
	CHBDYG / CONV / PCONV / MAT4	Convection
	QVOL	Internal heat generation
	TEMP	Ambient temperature
	TEMPD	Default nodal temperature
Contact	CONTACTGENERATE	Defines the default contact type and options. For bonded/welded contact with matched meshes, this card is not used. Instead nodes are merged where parts meet to establish the connection.
	BSCONP	Specifies the contact type (PTYPE) and options (such as friction) for explicitly defined contact pairs.
	BSSEG	Defines the two surface face segments
	PTYPE 1 through PTYPE 4 PTYPE 9 / PTYPE 10	Penetration type. The value of this parameter represents the following contact types. (This list includes all contact types supported for steady-state heat transfer analyses): 1: Unsymmetric general contact 2: Symmetric general contact 3: Unsymmetric welded contact 4: Symmetric welded contact 9: Unsymmetric offset welded contact 10: Symmetric offset welded contact
	MPC	Multipoint constraints (for smart bonded contact).
Thermal Solution Parameters	PARAM
	SIGMA	Stefan-Boltzman constant
	TABS	Scale factor for absolute temperature

Supported Result Types: Simulation Mechanical can translate the results to and from the NASTRAN OP2 file format.

The following results are translated from the NASTRAN file.

• Element heat flux vectors
• Element heat flux through surfaces with radiation or convection loads

The following results are translated to the NASTRAN file.

• Element heat flux vectors (not rod elements)
• Element heat flux through surfaces with radiation or convection load

General Notes:

In most cases, items in Simulation Mechanical are translated to NASTRAN equivalent elements. There are a few exceptions:

• Linear 2D plane stress and linear 2D plane strain elements are represented in NASTRAN using PSHELL / CQUADx / CTRIAx cards. Exporting axisymmetric 2D elements is not currently supported.
• Thick Composite elements are not supported by NASTRAN. When translated to NASTRAN, the geometry, material properties, and loads are translated to PCOMP / CQUAD4. Any core crushing properties are not translated.
• Rigid boundary elements are translated as CELAS2 in NASTRAN.
• Spring elements are translated as CONROD in NASTRAN. DOF spring elements are translated as CELAS2 in NASTRAN.
• Local coordinate systems are translated to CORD2R, CORD2C, and CORD2S in NASTRAN.

¹ Note: Pyramid elements are represented by CPYRAM cards in exported Nastran decks. When importing Nastran decks, CPYRA elements are accepted as equivalent to CPYRAM elements.