hmnasto2 Utility

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

To run hmnast02 independently, use the following syntax:

hmnasto2 [arguments] <inputfile> <outputfile>

where [arguments] are optional arguments. Arguments such as displacements, stresses, and strains are on by default. To obtain those arguments, use the command hmnasto2 -u.

To Run hmnasto2 From Hypermesh

1.	Open the Solver panel.

2.	Click the translator toggle and select hmnasto2.

3.	Click input file = and select the op2 file location and name.

4.	Click output file = and select the output file location and name.

5.	Enter the options.

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

The following options are off by default:

Flag	Meaning
-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
-linux	Linux
-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.

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, rotations, velocities and accelerations

•	Eigenvectors

•	Grid Point Stress

•	Nonlinear Stress and Strain

•	Element Name Codes: 90, 88, 85, 91, 93

•	Real and complex stresses

•	Element Name Codes: 4, 33, 39, 64, 67, 68, 74, 75, 144

•	Real strains

•	Element Name Codes: 4, 33, 39, 64, 67, 68, 74, 75, 144

•	Strain energies

•

Shear

•

Flux

How Displacement Results Translated by hmnasto2 are Displayed

MSC-Nastran writes displacement results into different data blocks based on selected parameters. When hmnasto2 reads these data blocks, a flag is set to 0 if it reads displacement results in basic* coordinate or 1 if it reads displacement result in global* coordinate. The -noconv option sets this flag to 0.

When HyperMesh reads the results file translated by hmnasto2, 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. If the value of the flag is 0, HyperMesh performs no further translation.

•	As defined by MSC-Nastran.

There are two ways to extract models (without result) from an op2 file:

1.	To extract a model in HMASCII format, use the following syntax:

hmnasto2 -<machine use to generate op2 file> <inputfile> <outputfile> <modelfile>

The model can be imported into HyperMesh using the HMASCII reader, which can be invoked from the import tab.

2.	To extract a model in h3d format, use the following syntax:

hmnasto2 -<machine use to generate op2 file> -h3d –model <inputfile> <modelfile>

The model can be imported into HyperView using the h3d reader.

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©.

•	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:

When STRESS(CORNER) is used, Nastran gives corner stresses on a per-element basis. However, hmnasto2 averages 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 modes and subcases, use the option -selsubc <selsubcfile> or -selmodes <selmodesfile>, where selmodesfile contains the mode numbers and selsubcfile contains the subcase numbers that need to be extracted.

How do I...

Post-process Nastran results in HyperMesh

Create an h3d file from HyperMesh

Create a model file from an op2 file and load the model file

Translating Complex Results

To Run hmnasto2 From Hypermesh

How Displacement Results Translated by hmnasto2 are Displayed

How do I...

See Also: