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:

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”

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

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)


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

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

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

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

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 ELEMENTS

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


HINGING/PINNING

Common problem when elements with different DOF’s are connected

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

 

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

EXAMPLE MATERIAL IN THE INPUT DECK


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.