liminfoNASTRAN Reference
Free reference guide: NASTRAN Reference
About NASTRAN Reference
The NASTRAN Reference is a searchable cheat sheet for structural analysts and FEA engineers working with MSC Nastran or NX Nastran. It provides complete bulk data card formats and field descriptions for geometry definition (GRID nodes with coordinate systems via CORD2R/CORD2C/CORD2S), 1D elements (CBAR constant-section beam, CBEAM variable-section with warping, CROD axial-only rod), 2D shell elements (CQUAD4 four-node quad, CTRIA3 three-node triangle, PSHELL property with membrane/bending/shear material IDs), and 3D solid elements (CHEXA 8/20-node hex, CTETRA, CPENTA, CPYRAM with PSOLID properties).
The material and loading sections cover isotropic material definition (MAT1 with E, G, NU, RHO, thermal expansion), anisotropic shell materials (MAT2 stiffness matrix, MAT8 orthotropic), concentrated forces (FORCE with magnitude and direction vector), surface pressure loads (PLOAD4 on element faces), gravity acceleration (GRAV requiring density in MAT1), temperature loads (TEMP/TEMPD), single-point constraints (SPC/SPC1 for fixed/pinned/roller boundaries), multi-point constraints (MPC linear equations), and rigid elements (RBE2 for stiff connections vs RBE3 for load distribution).
The solution sequence section covers the five most-used NASTRAN solutions with complete Case Control and Bulk Data setup: SOL 101 (linear static with displacement/stress/reaction output), SOL 103 (normal modes with EIGRL frequency extraction), SOL 105 (linear buckling with eigenvalue interpretation), SOL 111 (modal frequency response with FRF output), and SOL 200 (design optimization with DESVAR, DVPREL1, DRESP1, DCONSTR cards). Output request options (DISPLACEMENT, STRESS with VONMISES/CORNER, STRAIN) and essential PARAM cards (POST, AUTOSPC, COUPMASS, WTMASS, K6ROT) are also included.
Key Features
- GRID node definition with coordinate system options (CORD2R rectangular, CORD2C cylindrical, CORD2S spherical)
- 1D/2D/3D element reference: CBAR, CBEAM, CROD (1D), CQUAD4, CTRIA3, PSHELL (2D), CHEXA, CTETRA, CPENTA, PSOLID (3D)
- Material cards: MAT1 isotropic (steel/aluminum examples with E, NU, RHO) and MAT2 anisotropic for composites
- Load cards: FORCE (concentrated), PLOAD4 (surface pressure with THRU range), GRAV (gravity), TEMP/TEMPD (thermal)
- Boundary conditions: SPC/SPC1 (single-point constraints), MPC (multi-point equations), RBE2 vs RBE3 rigid elements
- Solution sequences: SOL 101 (static), SOL 103 (modes), SOL 105 (buckling), SOL 111 (frequency response), SOL 200 (optimization)
- Output requests: DISPLACEMENT, STRESS (VONMISES, BILIN, CORNER), STRAIN, SPCFORCES with SORT1/SORT2 and PRINT/PLOT options
- Essential PARAM cards: POST (-1 for OP2), AUTOSPC, COUPMASS, WTMASS (unit conversion), K6ROT (shell drilling stiffness)
Frequently Asked Questions
How do I define nodes and coordinate systems in NASTRAN?
Use the GRID card: GRID ID CP X1 X2 X3 CD PS SEID, where ID is the unique node number, CP is the coordinate system for input (0 = basic rectangular), X1/X2/X3 are coordinates, CD is the output coordinate system, and PS constrains DOFs (e.g., PS=123456 for fully fixed). Define local coordinate systems with CORD2R (rectangular), CORD2C (cylindrical), or CORD2S (spherical).
When should I use CQUAD4 vs CTRIA3 elements?
Always prefer CQUAD4 (4-node quad) as the primary shell element because CTRIA3 (3-node triangle) can exhibit overly stiff behavior. Use CTRIA3 only in mesh transition zones where quads cannot fill the geometry. Keep the triangle-to-total element ratio below 5%. For higher accuracy, consider CQUAD8 (8-node) or CTRIA6 (6-node) higher-order elements.
What is the difference between RBE2 and RBE3 elements?
RBE2 creates a rigid connection: the master (independent) node controls all slave (dependent) nodes, adding artificial stiffness to the model. Use it to simulate bolts, welds, or stiff connections. RBE3 distributes loads without adding stiffness: the reference node motion is interpolated from surrounding weighted nodes. Use it for applying loads over an area without artificially stiffening the structure.
How do I set up a linear static analysis (SOL 101)?
In Executive Control: SOL 101 / CEND. In Case Control: define SUBCASE with SPC (boundary condition set ID), LOAD (load set ID), and output requests (DISPLACEMENT=ALL, STRESS(VONMISES,BILIN)=ALL, SPCFORCES=ALL). In Bulk Data: define GRID nodes, elements (CQUAD4 etc.), properties (PSHELL), materials (MAT1), loads (FORCE/PLOAD4/GRAV), and constraints (SPC1).
How do I perform a modal analysis to find natural frequencies?
Use SOL 103 with METHOD card in Case Control pointing to an EIGRL card in Bulk Data. EIGRL specifies the frequency range (V1 to V2 in Hz) and number of modes (ND). For example: METHOD=10, then EIGRL 10 0.0 1000.0 20 extracts 20 modes between 0 and 1000 Hz. Output includes natural frequencies, mode shapes, and effective mass fractions.
How does buckling analysis (SOL 105) work?
SOL 105 requires two subcases: Subcase 1 applies the static load (SPC + LOAD), and Subcase 2 references Subcase 1 via STATSUB(BUCKLING)=1 with a METHOD card pointing to EIGRL. The eigenvalues represent buckling load factors: multiply applied load by the eigenvalue to get the critical buckling load. Eigenvalue > 1 means the structure is safe at the applied load level.
What unit system should I use in NASTRAN?
NASTRAN does not enforce units, so you must be consistent. Common systems: SI (N, m, kg, s) with E in Pa and RHO in kg/m3; or mm-based (N, mm, tonne, s) with E in MPa, RHO in tonne/mm3 (e.g., steel: E=210000, RHO=7.85E-9), and GRAV acceleration 9810. Use PARAM WTMASS for unit conversion if needed.
What are the most important PARAM cards?
PARAM POST -1 enables OP2 binary output for post-processing. PARAM AUTOSPC YES automatically constrains singular DOFs. PARAM COUPMASS 1 uses coupled (consistent) mass matrix instead of lumped. PARAM WTMASS converts mass units. PARAM K6ROT 100.0 adds drilling stiffness to shell elements. PARAM PRTMAXIM YES prints maximum values in the F06 file.