hmnasto2

Translates OUTPUT2 Nastran binary results into HyperMesh binary results files. hmnasto2 can be executed either independently or directly from HyperMesh.

Syntax

To run hmnast02 independently, use the following syntax:
hmnasto2 [arguments] <inputfile>
        <outputfile>

Application

Translators

Description

When you use hmnasto2, specify the machine used to generate the Nastran binary results file (-cray, -sgi or -pc, and so on). hmnasto2 supports the following data types:
  • Displacements, velocities and accelerations
  • Nonlinear Stress and StrainElement Name Codes: 90, 88, 85, 91, 93
  • Real and complex stressesElement Name Codes: 4, 33, 39, 64, 67, 68, 74, 75, 144
  • Real strainsElement Name Codes: 4, 33, 39, 64, 67, 68, 74, 75, 144
  • Strain energies
  • Shear
  • Flux

To extract displacements and maximum von Mises stresses from the OUTPUT2 file, use the option -d –von_max.

To extract only the maximum values of the data types, use the option -m.

For iterative solutions encountered in SOL 106, use the option -iter.

Simulation names:

hmnasto2 organizes the punch file results into series of simulation names and data types.

The simulation names correspond to the LABEL card for SOL101. The corresponding data types are displacements and von Mises stress, for example. If the option -nolabels is selected, the simulation name corresponds to the SUBCASE ID number.

The simulation name for SOL106 is 
SUBCASE # Iter
      #.
For modal frequency response problems, the simulation name is: 
Mode # f #Hz
For modal frequency response problems where the complex part of the eigenvalue is used (SOL 107 and SOL 110), the simulation name is:
Mode # f
      #Hz(c)
For direct frequency response, the simulation name is:
Subcase #f
      #
Do not use -nolabels for SOL106.
  • Corner options:

Use -corner option when STRESS(CORNER) or STRESS(BILIN) is used in the data file.

Note that when STRESS(CORNER) is used, Nastran gives corner stresses on a per-element basis. However, hmnasto2averages the corner stresses at the nodes for adjacent elements. If there is no geometry information in the op2 file, use an additional –bulk <bulkfilename> option. In general, geometry information is written into the op2 file if PARAM,POST,-2 is used in the input file. For more information regarding geometry information in an op2 file, see Nastran documentation.
  • If the size of the punch file is too large, use the option -disk -size n -file /temp/scratch.tmp, where n corresponds to the maximum number of nodes/elements in the model and scratch.tmp is the scratch file name that hmnasto2 creates in the /temp/ directory.
  • hmnasto2 supports OUTPUT2 files for the following solutions:
SOL 101, 103, 105, 106, 107, 108, 109, 110, 111 and 153.
  • hmnasto2 supports the following data block names for PARAM,POST,-1:
OQG1, OUGV1, OES1, OEF1, OSTR1, ONRGY1, OES1X and OPG1.
  • hmnasto2 supports the following data block names for PARAM,POST,-2:
OQG1, BOUGV1, BOPHIG, OUGV1, OES1, OEF1, OSTR1, ONRGY1, ONRGY2 and OES1X.
  • Use -nosubcman for SOL103 OUTPUT2 files when the HMNASTO2 default is unsatisfactory.
  • To extract only a selected set of nodes and subcases, use the option -selsubc <selsubcfile> or -selmodes <selmodesfile>. See hmnast for the file format.

Inputs

[arguments]
Optional arguments.
Arguments such as displacements, stresses, and strains are on by default.
Obtain these arguments using the command hmnasto2 -u.
-m
Displacements and maxs
-iter
Nonlinear iterations
-nolabels
Do not use subcase labels
-corner
Corner stresses
-csa
Translate CSA/Nastran
-subcman
Subcase manager
-cray
Cray
-dec
Dec 5000
-decalpha
Dec Alpha
-hp
Hewlett Packard
-ibm
IBM RS\6000
-pc
PC
-sgi
SGI
-sun
Sun
-h3d
Outputs file to an H3D file instead of an hmresults file. The file includes translated model and results information. The model must contain geometry for it to be output to an H3D file. If there is no geometry in the op2 file, use –bulk <filename> in addition to –h3d.
Example: 
hmnasto2 -h3d -bulk myFile.dat myFile.op2 myFile.h3d

H3D files can be created either by using hmnast or from HyperMesh.

Run hmnasto2 from HyperMesh

  1. Open HyperMesh.
  2. From the panel area, select the BC page.
  3. Click the Solver panel.
  4. Switch the toggle to hmnasto2.
  5. Click input file, and select the .op2 file location and name.
  6. Click output file, and select the output file location and name.
  7. Enter the options accordingly.
    Tip: The first option should be the machine used to generate the Nastran binary results file. To create an .h3d file for a specific result, add –h3d after the second option. For example, to create an .h3d file of the displacement result that was created from SGI computer, the option would be: -sgi -d –h3d
  8. Click solve.