|
»Click here to display Table of Contents«
|
hmnast Utility |
|
|
|
|
|
hmnast Utility |
|
|
|
|
|
»Click here to display Table of Contents«
|
hmnast Utility |
|
|
|
|
|
hmnast Utility |
|
|
|
|
hmnast translates Nastran ASCII punch files into HyperMesh binary results files. hmnast can be executed either independently or directly from HyperMesh.
hmnast [arguments] <inputfile> <outputfile>
where [arguments] are optional arguments. Arguments such as displacements, stresses and strains are on by default. To obtain these arguments, use the command hmnast -u.
| 1. | Open the Solver panel. |
| 2. | Click the translator toggle and select hmnast. |
| 3. | For input file:, click browse and select the punch file. |
| 4. | Click Open. |
| 5. | For output file:, click browse and select the output file location and name. |
| 6. | Click Open. |
| 7. | Enter the options. To create an h3d file for a specific result, add –h3d after the first option. For example, to create an h3d file of the displacement, the option should be -d –h3d |
| 8. | Click solve. |
The following options are off by default:
Flag |
Meaning |
-m |
Displacements and maximums |
-minimums |
Minimums instead of maximums |
-iter |
Nonlinear iterations (from SOL 106) |
-trans |
Transient thermal |
-corner |
Corner stresses (for CQUAD4 and solid elements) |
-bulk |
Reads element connectivity from the bulk file (for use with the corner option) |
-noconv |
Do not convert local displacements into global coordinates |
-nolabels |
Do not use subcase labels |
-title |
Use title for simulation name |
-subtitle |
Use subtitle for simulation name |
-disk |
Translation is performed on disk |
-size |
Number of entities (10000 = default) |
-file |
Scratch file name |
-csa |
Translates CSA/Nastran |
-1Dforce |
Reads all forces for 1-D elements |
-1Dstress |
Reads all stresses for 1-D elements |
-2Dforce |
Reads all forces for 2-D elements |
-repR |
Replaces R/NaN/nan fields with 0.0 (found in strain energy data types) |
-h3d |
Outputs file to an H3D file instead of an hmresults file. The hmresult file includes translated model and results information. The punch file must contain geometry for it to be output to an H3D file. If there is no geometry in the punch file, use –bulk <filename> in addition to –h3d. Example: hmnast -h3d -bulk myFile.dat myFile.pch myFile.h3d H3D files can be created either by using hmnast or from HyperMesh. |
hmnast supports the following data types:
Displacements, rotations, velocities, and accelerations
SPC forces and SPC moments
Grid Point Force Balance (totals block only)
Real element forces
Element name codes: 1, 2, 10, 11, 12, 33, 34, 74, 100
Real stresses
Element name codes: 1, 2, 4, 10, 33, 34, 39, 64, 67, 68, 70, 74, 75, 82, 85, 88, 90, 91, 93, 144
Real strains
Element name codes: 4, 33, 39, 64, 67, 68, 70, 74, 75, 82, 85, 88, 90, 91, 93, 144
Complex stresses
Element name codes: 33, 39, 64, 67, 68, 70, 74, 75, 82
Complex strains
Element name codes: 33, 39, 64, 67, 68, 70, 74, 75, 82
Temperatures
Flux
Strain energies
Time
Eigenvectors
Frequency
When hmnast reads displacement results, a flag is set to 1. The -noconv option sets this flag to 0.
When HyperMesh reads the results file translated by hmnast, it checks the value of the flag. If the value is 1, HyperMesh translates the nodal displacement into basic* coordinate using the system attached to the node, in the case where no system is attached to the node, HyperMesh performs no further translation. If the value of the flag is 0, HyperMesh performs no further translation.
| • | As defined by MSC-Nastran. |
To extract displacements and maximum von Mises stresses from the punch file, use the option -d -von_max.
To extract only the maximum values of the data types, specify the option -m.
For iterative solutions encountered in SOL 106, use the option -iter.
For transient solutions encountered in SOL 159, use the option -trans.
For nonlinear transient solutions encountered in SOL 129, use the options -trans -iter.
Corner stresses:
| • | Use -corner option when STRESS(CORNER) or STRESS(BILIN) is used in the data file. |
| • | When using -corner option, hmnast requires the bulk data information. This can be done by using ECHO=PUNCH during analysis. Otherwise, use the -bulk <bulkfilename> option. |
| • | When using STRESS(CORNER), Nastran gives corner stresses on a per-element basis. However, hmnast averages the corner stresses at the nodes for adjacent elements. |
HyperMesh converts the nodal displacements into global coordinates if there are non-zero values in the CD field of the GRID cards. To display the results in HyperMesh as they are reported in the punch file, use the option -noconv
Simulation names:
| • | hmnast organizes the punch file results into a series of simulation names and data types. The simulation names correspond to the LABEL card of the punch file for SOL101. To create a simulation name, the first 27 characters from the LABEL card are appended with the SUBCASE ID. The corresponding data types are Displacements, von Mises Stress, and so on. If the option -nolabels is selected, the simulation name corresponds to the SUBCASE ID number. |
| • | Use -title to use the TITLE card of your punch file as the simulation name. |
| • | Use -subtitle to use the SUBTITLE card of your punch file as the simulation name. |
| • | 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©. |
| • | For direct frequency response, the simulation name is Subcase # f #. |
| • | For transient problems (SOL159, SOL129), the simulation name is Time #. |
Do not use -nolabels for SOL106, SOL159, and SOL129.
| • | 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 hmnast creates in the /tmp/ directory. |
| • | hmnast supports punch files for the following solutions: SOL 101, 103, 105, 106, 107, 108, 109, 110, 111, 112, 129, 153 and 159 |
| • | To extract only selected modes from a punch file, use the option -selmodes <selmodesfile>, where selmodesfile contains the mode numbers that need to be extracted. These numbers must have spaces separating them. Any number of lines can be entered. A line cannot exceed 256 characters. To extract only a selected number of subcases, use the option -selsubc <selsubcfile>. |
Post process Nastran results in HyperMesh
Create an h3d file from HyperMesh