NASTRAN

Autodesk Simulation will import and export models in the MSC.Nastran format.

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 Autodesk Simulation items are translated to the NASTRAN input file with the exceptions listed below the table.

	NASTRAN	Autodesk Simulation
Truss Elements	PROD/CROD or CONROD	Linear truss
Beam Elements	PBAR/CBAR	Linear beam (offsets and end releases will also be transferred from CBAR)
	PLOAD1	Linear beam distributed loads
	PBEAM/CBEAM	Linear beam with constant cross-sectional properties (the first set of cross-sectional properties will be used)
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)
	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	PSOLID/CHEXA/CPENTA/CTETRA	Linear brick (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.
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: Autodesk Simulation 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

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 Autodesk Simulation items are translated to the NASTRAN input file with the exceptions listed below the table.

	NASTRAN	Autodesk Simulation
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	PSOLID/CHEXA/CPENTA/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

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

The following results will be translated from the NASTRAN file.

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

The following results will be translated to the NASTRAN file.

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

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 Autodesk Simulation items are translated to the NASTRAN input file with the exceptions listed below the table.

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

Result Types Supported: Autodesk Simulation 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

In most cases, items in Autodesk Simulation will be translated to NASTRAN. There are a few exceptions:

• If a brick model in Autodesk Simulation contains pyramids (5-noded elements), they will be split into 2 tetrahedral elements when translated to NASTRAN. This will also occur if a model is solved in Autodesk Simulation using the NASTRAN solver.
• 2D elements are not supported by NASTRAN. When translated to NASTRAN, the geometry, material properties and loads will be translated to PSHELL/CQUAD4.
• Thick Composite elements are not supported by NASTRAN. When translated to NASTRAN, the geometry, material properties and loads will be translated to PCOMP/CQUAD4. Any core crushing properties will not be translated.
• Rigid boundary elements will be translated as CELAS2 in NASTRAN.
• A spring element will be translated as CONROD in NASTRAN. A DOF spring element will be translated as CELAS2 in NASTRAN.
• Local coordinate systems will be translated to CORD2R, CORD2C and CORD2S in NASTRAN.
• If a model contains linear contact, the contact elements will be translated to PGAP and CGAP cards. A rectangular coordinate system will also be created for each element to define the axial direction.
• If a model contains thermal contact, the thermal contact elements will not be exported.

Parent topic: FEA Model Import and Export Functionality