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 (MSC 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) |
| 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 | PTYPE 1 / PTYPE 4 / PTYPE 9 | These NASTRAN cards represent symmetric general contact (for linear surface contact in Simulation Mechanical), bonded contact (RBE3), and symmetric welded contact, respectively. |
BSSEG |
Defines the two surface face segments |
|
BSCONP |
Ties two surfaces together and specifies the penetration options and parameters (such as friction). |
|
| 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 and material models 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 an MSC 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 2 | Symmetric general contact. |
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 | PTYPE 2 | Symmetric general contact with thermal resistance. |
BSSEG |
Defines the two surface face segments |
|
BSCONP |
Ties two surfaces together and specifies the parameters (such as thermal resistance). |
|
| MPC | Multipoint constraints (for smart bonded contact). |
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:
- 2D elements are not supported by NASTRAN. When translated to NASTRAN, the geometry, material properties and loads are translated to PSHELL / CQUAD4.
- 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.