Output Controls

The controls of the Output Controls category vary based on the type of analysis being performed.

Output Controls give you the ability to specify which type of quantities are written to the result file for use during post-processing. As a result, you can control the size of the results file which can be beneficial when performing a large analysis.

The following Output Controls are available in the Details view to be activated (Yes) or not (No) and included or not included in the results file. Note that these controls are not step-aware, meaning that the settings are constant across multiple steps.


Note:
  • It is recommended that you not change Output Controls settings during a Solution Restart. Modifying Output Controls settings change the availability of the respective result type in the results file. Consequently, result calculations cannot be guaranteed for the entire solution. In addition, Result file values may not correspond to GUI settings in this scenario. Settings turned off during a restart generate results equal to zero and may affect post processing of results and are therefore unreliable.

  • Modification of Stress, Strain, Nodal Force, Contact Miscellaneous, and General Miscellaneous properties will not invalidate the solution. If you want these Output Controls settings modifications to be incorporated to your solution, clean the solution first.


Multiple Step Properties

In addition, the following settings are step-aware and allow you to define when data is calculated and written to the result file for Static Structural, Transient Structural, Rigid Dynamics, Steady-State Thermal, Transient Thermal, and Topology Optimization analyses:

Recommended Settings for Modal and Linked Analysis Systems

The following table provides a summary of recommended settings for Store Modal Results and Expand Results From based on the analysis type.

Analysis TypeRecommended Store Modal Results SettingsRecommended Expand Results From Settings
Modal with no downstream linked analysis

No

Stress and strain results not needed to be saved to file.mode because there is no downstream analysis.

Not available.
MSUP Harmonic Response analyses (Linked and Standalone)

No

Stress and strain results from modal analysis are overwritten by stresses and strains which are expanded again in the linked Harmonic Response analysis due to any loads added in the downstream analysis.

Note:  This setting is available for a linked MSUP Harmonic Response analysis only.

Harmonic Solution

Use when number of frequency steps are far less than the number of modes. This option is not available when the Modal has a nonlinear Pre-Stress environment.

Modal Solution

Use when number of frequency steps are far more than the number of modes. This is the only option available when the Modal analysis has a nonlinear Pre-Stress environment.

Modal with downstream linked Random Vibration analysis

For Future Analysis

Stress and strain results from modal analysis are expanded and used in the linked random vibration analysis. No stress or strain expansion is needed again because there is no load.

Not available.
Modal with downstream linked Response Spectrum analysis

No

Stress and strain results are always combined in response spectrum analysis using file.rst and file.mcom.

Note:  To evaluate summation of element nodal forces using FSUM in Command Snippet, it is required to save element nodal forces in modal to file.mode.

Not available.
Modal with downstream linked Topology Optimization

For Future Analysis

The Nodal Forces and the General Miscellaneous properties are set to Yes.

Program controlled.
Static Structural with downstream linked Topology Optimization

For Future Analysis

The Nodal Forces property is set to Yes.

Program controlled.
Modal with downstream linked Transient analysis

No

Stress and strain results from modal analysis are overwritten by stresses and strains which are expanded again in the linked transient analysis due to any loads added in the downstream analysis.

Transient Solution

Use when number of time steps accumulated over all the load steps is far less than the number of modes.

This option is not available when the Modal Analysis has a nonlinear Pre-Stress environment.

Modal Solution

Use when number of time steps accumulated over all the load steps is far more than the number of modes.

This is the only option available when the Modal Analysis has a nonlinear Pre-Stress environment.

Limitations When Using the Mechanical APDL Solver


Release 18.2 - © ANSYS, Inc. All rights reserved.