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
    • 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

  • 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

  • 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)

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


  • Rigid element
  • Infinitely stiff
    • Adds stiffness to model
  • No mass

  • 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

  • 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



  • 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 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


Example Constraint 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.

Have a problem we can solve?

Who We Are

Quartus Engineering specializes in system design & development, simulation & analysis, testing, prototyping and manufacturing of mechanical systems for a wide-range of industries and are experts in simulation-driven engineering. We are a complete engineering solution provider from concept, prototype through low volume or complex production. We design for manufacturability and transition to high volumes with ease with Quartus as your guide. Quartus has depth and broad range of industry and product experience that includes: Civil/Space, Defense, Aircraft/Transportation, Consumer Products, Optics & Photonics and Medical/Life Science. Quartus is focused on game changing applications like remote sensing, metrology, thermal, LiDAR, use of novel materials and other innovative technologies and measurement approaches that span multiple industries and are faced with extreme environments and other complex engineering challenges.

SAN DIEGO 9689 Towne Centre Dr San Diego, California 92121 T (858) 875-6000   MORE INFO
HERNDON 2300 Dulles Station Blvd Suite 650 Herndon, Virginia 20171 T (571) 266-5300 MORE INFO