NASTRAN User Guide

  1. Home
  2. Reference
  3. NASTRAN User Guide

nanstran1

OUTLINE

  • Introduction
  • File Structure
  • Executive Control
  • Bulk Data
  • Element Types
  • Element Examples
  • Output Files

WHAT IS A FINITE ELEMENT ‘SOLVER’?

  • NASTRAN is one of many available finite element analysis (FEA) solvers
    • Other solvers at Quartus: 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 commonly used with NASTRAN

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)
  • Today there are many flavors (or versions) of Nastran MSC, NX, etc.

Nastran at Quartus

  • Primary program used for finite element analysis
  • Used extensively to perform static, buckling, and dynamic analyses of structures
  • Quartus has licenses for both NX/Nastran and MSC Nastran
    • Largely the same (basic functionality)
    • Some small differences and enhancements

WHAT UNITS DOES NASTRAN USE?

  • NASTRAN does not have a defined unit system
  • The user must be careful to maintain consistent units Units must be consistent such that units satisfy F= ma Examples for English and SI units are shown below:

nanstran2

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/sec^2)

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

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”

nanstran3

nanstran4

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

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

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

SOL – COMMON SOLUTION SEQUENCES

nanstran5

EXECUTIVE CONTROL – EXAMPLE INPUT DECK

Executive Control Section in the example deck:

nanstran6 1

This example deck performs a “normal modes” analysis.

SOL 103 = SOL SEMODES (either way will work)

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

nanstran7

MAIN PARTS OF BULK DATA

  • Nodes
  • Elements
  • Coordinate Systems
  • Properties
  • Materials
  • Constraints
  • Analysis Parameters (PARAM, . . . )

BULK DATA: FORMAT

The bulk section is not order dependent. There are 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

INPUT DECK NODE EXAMPLE

nanstran8

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

nanstran9

1D ELEMENTS

Common element types: beams, bars, rods

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

2D ELEMENTS

Common element types: plates, laminates, membranes

nanstran10

DOF

  • 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

3D ELEMENTSnanstran11

Common element types:

  • Solids
    • Shapes: bricks (CHEXA), wedges (CPENTA), tetrahedrons (CTETRA)

DOF

  • 3D element nodes have associated stiffness in 3 DOF (T1, T2, and T3)

R-TYPE

RBE2

  • 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

CONNECTOR / OTHER ELEMENTS

Common element types: Springs, Lumped Masses

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

INPUT DECK ELEMENT EXAMPLE

nanstran12

HINGING/PINNING

Common problem when elements with different DOF’s are connected

  • Plates to Solids
  • Beams and Bars to Plates or Solids

nanstran13

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

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

EXAMPLE PROPERTY IN THE INPUT DECK

nanstran14

EXAMPLE MATERIAL IN THE INPUT DECK

nanstran15

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.