1. Nastran 101
February 28, 2008

2. What is a Finite Element ‘Solver’?
NASTRAN is one of many available finite element analysis (FEA) solvers
Other solvers: ABAQUS, ANSYS, LS-DYNA
What does a solver do? (the short answer)
User provides input in the form of a text file
Solver reads the text file and performs analysis
The solver generates output files with analysis results
How does the user make the input text file?
Models are created and input files exported using FEA pre/post processing software
Various Pre/Post Processors available
FEMAP, PATRAN, and Hypermesh are commonly used with NASTRAN

3. What is Nastran?
Nastran is a powerful finite element analysis program that is used widely in the aerospace and automotive industries
Industry standard finite element code originally developed for NASA by MSC (1960s)
Current industry standard structural FEA code for spacecraft, launch vehicles, linear structural dynamics, etc.
Today there are many flavors (or versions) of Nastran
MSC, NX, etc.
Continued maintenance and enhancement

4. What Units Does NASTRAN Use?
Nastran does not use a unit system
The user must be very careful to maintain consistent units
Units must be consistent such that units satisfy F= ma
Examples for English and SI units are shown below:
Note: for English units (in, lbf, sec), the unit of mass is a ‘slinch’ (lbf-sec2/in), not a pound (lb). A slinch is the ‘inch version of a slug’. To convert from pounds to slinches you divide by the acceleration of gravity (386.1 in/sec2)

5. What is an Input File?
At the most basic level, it’s nothing more than a formatted text file
Defines the finite element model and all parameters necessary for analysis
Nastran input files are often referred to as ‘decks’
Origin of terminology comes from the time when the data was stored on actual punch cards and then fed into a machine that would read the ‘deck’ of cards.
File extensions vary
.dat usually used for input files
.blk or .bdf usually used for included files
Common text editors
EditPad, UltraEdit, EmEditor, Emacs

6. What’s in a Nastran Input Deck?
Every deck can have 5 main sections
Nastran statement
File management statements (FMS)
Executive control statements
Case Control commands
Bulk Data entries
The format and definition for all entries in the input deck can be found in the NASTRAN quick reference guides
Commonly referred to as “the NASTRAN bible”

7. Example Deck Executive Control statements Case Control commands
Bulk Data entries

8. NASTRAN Statement This section is optional
This section is usually used only on large jobs where modifications are needed to more effectively run the job
Used to change parameters for the solve
BUFFSIZE
DMP
Scratch file setup

9. File Management Section
This section is optional
File management section is used primarily for saving databases and setting up restart files
Restart a job from a previously analyzed job to reduce solve times

10. Executive Control Section
Executive control section is required for all runs
Includes:
DMAP control Section (optional)
ID (optional)
Identification for the Job
SOL (required)
What type of solution? (linear static, buckling, modes, etc.)
ECHO (optional)
Control whether the executive control section is output to file
Time (optional)
Set up max CPU time
DIAG (optional)
Options for diagnostic information

11. SOL – Common Solution Sequences
101
SESTATICS
Linear statics
103
SEMODES
Normal Modes
105
SEBUCKL
Static Linear Buckling
106
NLSTATIC
Nonlinear statics
Linear statics with Gaps
108
SEDFREQ
Direct Frequency Response
109
SEDTRAN
Direct transient response
111
SEMFREQ
Modal frequency response
112
SEMTRAN
Modal transient response

12. Executive Control – Example Input Deck
Executive Control Section in the example deck:
This example deck performs a “normal modes” analysis
SOL 103 = SOL SEMODES (either way will work)

13. Case Control Section Case control section is required for all runs
Common features:
Selection of constraint set (SPC)
Selection of load set (LOAD)
Selection of eigenvalue extraction parameters (METHOD)
Used for buckling, modes, frequency response
Output requests
Example:
Output all nodal displacements
Output all constraint forces
Output all element strain energy
Identifies set ID for eigenvalue extraction parameters
Selects active constraint set (1)

14. Main Parts of Bulk Data Nodes Elements Coordinate Systems Properties
Materials
Constraints
Analysis Parameters (PARAM, )

15. Bulk Data: Format The bulk section is not order dependent
3 options for format (can use each type within a single deck)
Tab delimited
Space delimited (default, short-field format = 8 spaces / field)
Decks written from FEMAP and Hypermesh are space delimited
Comma delimited

16. Input Deck Node Example
From the NASTRAN bible
From the example input deck

17. Element Information 5 major types of elements 1D Elements Bars Beams
Rods
2D Elements
Plates
Laminates
3D Elements
Solids
R-Type (rigids)
RBE2
RBE3
Connector / Other Elements
Springs
Lumped Masses

18. 1D Elements Common Element Types DOF
Bars and Beams have axial, shear (2), bending (2), and torsion stiffness
Bars and beams are basically the same
Beams have more options
Rods only have axial and torsion stiffness
Beams
Bars
Rods

19. 2D Elements DOF Common Element Types Plates
Laminates
Membranes
Plates and Laminates have in-plane (2), shear (in-plane and transverse), and bending stiffness
Stiffness is associated with attached nodes for DOFs T1, T2, T3, R1, and R2
No ‘drilling’ (R3) stiffness
Membrane elements only have in-plane (normal) stiffness

20. 3D Elements DOF 3D element nodes have associated stiffness in 3 DOF
Common Element Types
DOF
Solids
Shapes: bricks (CHEXA), wedges (CPENTA), tetrahedrons (CTETRA)
3D element nodes have associated stiffness in 3 DOF
T1, T2, and T3

21. R-Type RBE2 RBE3 Nodes on RBE’s are either dependent or independent
Rigid element
Infinitely stiff
Adds stiffness to model
No mass
RBE3
Interpolation elements (constraint equations)
Used to ‘average’ the responses of a number of nodes
Does not add stiffness to model
Nodes on RBE’s are either dependent or independent
Important to be aware of dependencies
Cannot apply boundary conditions to dependent nodes
Nodes cannot be dependent on more than 1 RBE

22. Connector / Other Elements
Common Element Types
DOF
Springs are normally used to connect coincident nodes
Connect elements
Recover forces
Two main types of spring elements
CELASi: connects only 1 DOF
Multiple elements are required to connect more than 1 DOF
CBUSH: can connect 1-6 DOF
Newer, more versatile spring element
Lumped masses are used to model mass and inertia at a node and have no stiffness
CONMi
Springs
Lumped Masses

23. Input Deck Element Example
From the NASTRAN bible
From the example input deck

24. Hinging / Pinning
Common problem when elements with different DOF’s are connected
Plates to Solids
Beams and Bars to Plates or Solids
Although the plate grids have rotational (bending) stiffness, the grids on the solid do not. Therefore, at the plate to solid interface no moments can be transferred into the solid, creating a hinge
Solution: overlap the solids with the shell by a minimum of one element
Plate Grids has 5 DOF
Solid Grids have 3 DOF

25. Coordinate Systems
Coordinate systems are used to define node locations and output
Nodes can have different definition and output coordinate systems
Coordinate system zero is the default rectangular system located at (0,0,0)
Rectangular, cylindrical, and spherical coordinate systems can be used in Nastran

26. Properties Properties define the characteristics of the elements
Plate thickness, beam cross-section, spring stiffness, etc.
Properties reference materials
Materials are defined on separate cards
Each element type has a different property
Some elements don’t use a property but instead input the information directly on the element card

27. Example Property in the Input Deck
From the NASTRAN bible
From the example input deck

28. Example Material in the Input Deck
From the NASTRAN bible
From the example input deck

29. Example Constraint in the Input Deck
From the NASTRAN bible
From the example input deck

30. Nastran Files: Common Output Files
.op2
Output2 File: binary file including results for FEMAP
Most commonly used file for output
.pch
Punch File: results in tabulated text format
.f06
Text file with results from analysis along with diagnostic messages
Can be read by FEMAP or processed by various custom programs
.f04
Text file containing run information; database file info, module execution summary, etc. (highly detailed log)
.log
Text file with general information; control file info, run time, licensing information, etc.