HyperMesh and BatchMesher

To specify output options:

To specify output options:

 Previous topic Next topic No expanding text in this topic  

To specify output options:

 Previous topic Next topic JavaScript is required for expanding text JavaScript is required for the print function  

The Output Options section contains various options to review and display the results of Resultant Force and Moment extractions.

1.Use the Coordinate System selector to determine the coordinate system used to output the nodal coordinates (x,y,z) in the summary table, .csv file, and .fbd file output options.

Resultant force and moment vector results are always output in the result coordinate system defined for each cross-section.  Result coordinate systems for cross-sections are defined using the Cross-section Manager.  If a coordinate system is not specified, the HyperMesh "base" system is used by default.

The Resultant Force and Moment utility extracts grid point force and moment results from the results file in the output coordinate system in which the solver output these results.  It is assumed that the output coordinate system assigned to each node in the database matches that used to run the analysis and generate the results file.  Output coordinate systems are defined by accessing the Systems panel.  (On the assign subpanel, select the required nodes and a coordinate system, and click Set Analysis.  In OptiStruct and Nastran this operation sets the CD field on the GRID cards).

If the output coordinate systems for each node in the database do not match those used to run the analysis, the extracted values will be incorrect.  This can occur when modifying nodal output system without rerunning the analysis, and/or loading a results file that does not match the currently loaded model.  In addition, results coming from or output to cylindrical or spherical result coordinate systems should be inspected for validity near the origin and along principal axes.

MPC force and moment data are properly extracted for the following MPC constraint types: RBE2, RBE3, Rigidlink, RJOINT, RROD, RBAR.

2.Use the Zero Tolerance field to specify the cut-off point below which a result quantity is considered zero.

All calculations are done with float point precision and the zero tolerance value is only used to control the output of results to the various formats.  The option helps to eliminate relatively small values from being output.  To maintain float precision the default is set to 1.0e-6, otherwise modify the value as desired.

3.Activate the Create Load Collectors checkbox to extract the specified grid point data and display it in organized load collectors for graphical visualization within the model window.

Multiple load collectors are created — one for each force and moment component — for each selected loadstep of the current cross-section, each made up of an element set and node set.  The load collector name format is "RF&M_E(#)_N(#)_S(#)_(compID)".  For example RF&M_E(1)_N(1)_S(1)_Fx would be created for element set 1, node set 1, loadstep 1, and component Fx.

The "Color" option allows you to choose a color for all created load collectors.  This color can be modified later using either the interface or the FBD Results Manager.

You can also use the FBD Results Manager to review the load collectors generated from the Resultant Force and Moment utility.  When the database is saved, all resultant force and moment load collectors are saved in the database.  This allows resultant force and moment information to be reviewed and utilized in the future without having to rerun the tool.  Renumbering element or node sets after running the tool invalidates the link between the load collector names and the associated sets and therefore it is important to not renumber any element or node sets for which resultant force and moment result are to be retained as load collectors in HyperMesh.

4.Activate the Show summary table option to output the results to a popup window for instant review.

The table contains information about the loadsteps and cross-sections, and detailed data from the grid point extraction at each node.

5.Activate the Create .csv file option to create a .csv file containing the same information as the summary table, but in a comma separated file.

You may select a new file or an existing file.  If an existing file is selected, it is appended to.

6.Activate the Create .fbd file option to create a file that can be read into HyperGraph using the "Shear and Moment Plot" and "Potato Plot" utilities.

You may select a new file or an existing file.

 

Comments

When saving over existing .csv or .fbd file, there are several items to note:

•If the data you are extracting already exists in the file (based on element set, loadstep IDs), the existing block will be overwritten with the new data.  If it does not exist, it will be appended to the end of the file.
•You are asked if you wish to replace the existing file.  However, selecting ‘yes’ will not overwrite the file; it will append/replace the data into the file as described above.
•Two utilities available within HyperGraph interact with data generated from the Resultant Force and Moment utility: Shear and Moment Diagrams (VMT Plots) and Potato Plot.  These utilities are accessed from the Free Body Diagrams item within the HyperGraph Utilities menu.