Solution

Number of Sectors: For an analysis that includes a Cyclic Region, this value indicates how many sectors should be processed, displayed and animated. Results generate more quickly and consume less memory and file storage when fewer sectors are requested. The default setting is Program Controlled (0).

Starting at Section: For an analysis that includes a Cyclic Region, selects the specific sectors to include within the expansion. For example, if Number of Sectors property is set to 1, sectors 1 through N are revealed one at a time. The default setting is Program Controlled (0).

Post Processing

Beam Section Results (Line Bodies Only): Options include Yes and No (default). This property enables you to choose whether to display beam results using expanded data when you specify your line body model as a beam/pipe that includes cross sections (SECDATA). This means that the application displays beam results with realistic contours that can vary along all coordinates and display stress and strain results as well as deformations, such as torsional rotation. Displaying unexpanded results reduces the amount of storage required for the result, however, the application displays the beam contour results using constant radial values. As a result, the setting of the property directly affects the results values displayed on your model.

Note:

The application always uses expanded results when displaying animations.
Probe annotation labels always display expanded results.

Frequency Display (Modal Analyses Only): Displays when the Solver Type property (Analysis Settings) is set to Full Damped. Options for this property include Program Controlled (default) and All. Setting the property to All enables the results evaluation to be carried out on all the frequencies extracted from the modal solution (that may or may not be conjugate pair). This process increases the number of results sets and listings of the frequencies in the Tabular Data window even if you request a lower number of modes. When set to Program Controlled, the results evaluation treats complex frequencies as complex conjugate pairs.

Note: The Tabular Data window can display negative frequencies when the solver reports nonconjugate pairs of complex frequencies. Setting the Frequency Display property to All displays all complex frequencies. This enables you to specify results at desired frequencies.

On Demand Stress/Strain: Supported for Static Structural analyses only. The options include Yes and No (default). This property generates element nodal stress, elastic strain, and thermal strain results without writing the associated data to the result (.rst) file. When you request results to be evaluated with this option, the application calculates these result quantities using the displacements available in the result file. This feature enables you to minimize the size of the result file while also reviewing results. However, the processing requirements are slowed.

Recommendations

Review the following recommendations for the use of the On Demand Stress/Strain property:

Set the Stress and Strain properties of the Output Controls of the Analysis Settings object to No.
If you apply Thermal Conditions in order to calculate Thermal Strains, you should set the Nodal Forces property (Output Controls > Analysis Settings) property to Yes.
If you have performed a solution with this property set to No, you should clear any generated data prior to changing the property to Yes in order to establish clean data.
To display Structural Error results, set the General Miscellaneous property (Analysis Settings > Output Controls) to Yes.

Limitations

Review the following limitations for the use of this feature:

It cannot display Elemental Euler Angle results.
Result evaluation slows considerably when you set the Calculate Time History property to Yes for a result in a multistep analysis.
The application does not support Stress, Elastic Strain, and Thermal Strain for tapered shell models.
Stress and Strain results are not supported for line bodies defined with pipe elements.

During a Structural Optimization in Mechanical, the application displays the following additional properties in the Post Processing category:

Export Optimal Shape

You can further analyze your optimized model, through continued simulation or by performing a design validation by exporting your results and making them available to a new downstream system.

The Export Optimal Shape property enables you to automatically export your results in Standard Tessellation Language (STL) and in Part Manager Database (PMDB) file format, archive the files in zip file format, and then place the zipped file in the Solver Files Directory. This option is set to Only Geometry by default.

In order to make the optimized results available to a downstream system, you need to create the new system on the Workbench Project Schematic and link the Results cell of your Structural Optimization analysis to the Geometry cell of a new downstream system, either a Geometry component system or the Geometry cell of another analysis system. Refer to the Design Validation section for additional details about this process.

Topology Result

When the Export Optimal Shape property is set to Only Geometry, the Topology Result property also displays. The No setting removes this property form the Details view. The Topology Result property provides a drop-down of available Topology Density results. For the Structural Optimization Environment, the Topology Result property includes a default selection.

Definition (Structural Optimization only)

Environment Selection List: Read-only property that points to the upstream analysis system (system cell ID) being used for the solution in your Structural Optimization analysis. You may use the options available in the property to select a different upstream system.

Tree Dependencies

Valid Parent Tree Object: Any Environment object.
Valid Child Tree Objects: All general Results and Result Tools, Commands, Comment, Figure, Image, and Solution Information.

Insertion Methods

This object displays by default for any analysis.

Note: A Solution object cannot be deleted from the tree.

Right-click Options

In addition to common right-click options, relevant right-click options for this object include:

Insert >
- [supported result types]
- Commands
- Python Code
Solve
Get Results: Available only for a completed solution on a remote machine.
Note: For a solution completed using the Ansys Remote Solve Manager (RSM), ff you have the RSM Output Files Download preference set to Show, the RSM File Manager dialog displays, and enables you to select or clear the input/output files you wish to download. See the Results category of the Options dialog to change this preference. The default setting is to hide this dialog. The dialog displays with certain files selected by default. See the Solving section for more information.
Evaluate All Results
Stop Solution: Available only for remote solutions.
Interrupt Solution: Available only for remote solutions.
Export Nastran File
Clear Generated Data
Group All Similar Children
Open Solver Files Directory
Reload Result File: This option is visible when you are using the By Reference option of the Read Result Files feature. It enables you to re-read the selected result files and reevaluate the solution.
Worksheet: Result Summary: Available following the completion of the solution process. This option displays the results content in a tabular format.

API Reference

See the Solution section of the ACT API Reference Guide for specific scripting information.

Additional Related Information

See the following sections for more information: