hmnast
Translates Nastran ASCII punch files into HyperMesh binary results files. hmnast can be executed either independently or directly from HyperMesh.
Syntax
hmnast [arguments] <inputfile>
<outputfile>
Application
Translators
Description
- 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
- 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.
- 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.
Mode # f
#Hz(c).
Subcase # f
#.
For transient problems (SOL159, SOL129), the simulation name isTime #.
- 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 nodes 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>.
Inputs
[arguments] are optional arguments. Arguments such as displacements, stresses and strains are onby default. To obtain these arguments, use the command hmnast -u.
- -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 1D elements
- -1Dstress
- Reads all stresses for 1D elements
- -2Dforce
- Reads all forces for 2D 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.
Example
N/A