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 () or not () 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.
Stress. Writes element nodal stresses to the results file. The default value is . Available for Static Structural, Transient Structural, Modal, and Eigenvalue Buckling analysis types.
Strain. Writes element elastic strains to the results file. The default value is . Available for Static Structural, Transient Structural, Modal, and Eigenvalue Buckling analysis types.
Nodal Forces. Writes elemental nodal forces to the results file. Options include:
: No nodal forces are written to the results file. This is the default setting except for a Modal Analysis in which the Future Analysis property, under Analysis Data Management category, is set to . In that case, the default setting is .
: This option writes nodal forces for all nodes. It is available for Static Structural, Transient Structural, Harmonic Response, Modal, Steady-State Thermal, and Transient Thermal analysis types. This Output Control must be set to if you want to use the Mechanical APDL Command NFORCE, FSUM in Mechanical (via command snippets) because those MAPDL commands will access nodal force records in the result file as well as to obtain Reactions on the underlying source or target element. For thermal analyses, nodal forces represent heat reactions.
If Future Analysis property, under Analysis Data Management category, is set to , , or , then the Nodal Forces property is automatically set to and becomes read-only.
. This option writes nodal forces for constrained nodes only. It is available for a Modal Analysis as well as Mode-Superposition (MSUP) Harmonic Response and Transient analyses that are linked to a Modal Analysis with the option set to the . This option directs Mechanical to use only the constrained nodes when calculating reaction forces and moments. The advantage is a reduced results file size.
Calculate Reactions. Turn On for Nodal Forces on constraints. Available for Modal, Harmonic Response, and Transient (applicable only when linked to a Modal analysis.) analysis types.
Calculate Velocity and Acceleration. Writes Velocity and Acceleration results to the result file. The default value is . Available for Mode-Superposition (MSUP) Transient Structural analyses only.
Calculate Thermal Flux. Available for Steady-State Thermal and Transient Thermal analysis types.
Keep Modal Results. Available for Random Vibration analyses only. The default value is . This setting removes modal results from the result file in an effort to reduce file size. Setting this property to allows you to perform post-processing on results of the Random Vibration solution (e.g., Response PSD) via command snippets.
Calculate Velocity. Writes Velocity to the results file. Available for Response Spectrum and Random Vibration analysis types. The default value is for both analysis types.
Calculate Acceleration. Writes Acceleration to the results file. Available for Response Spectrum and Random Vibration analysis types. The default value is for both analysis types.
Contact Miscellaneous. Turn On if Contact Based Force Reactions are desired. The default value is . Available for Static and Transient Structural analysis types. Not Available when linked to a Modal analysis.
Participation Factor (Modal Analysis Only). This property displays when the Solver Type (in Solver Controls category) property is set to . The options for this property include:
(default): When selected, the application automatically provides the Participation Factor Summary based on the following criteria.
If the Future Analysis property of the Analysis Data Management category is set to , the application creates the file, file.full, and the option becomes available in the drop-down list for the Solution Output property (under the Solution Information object).
If the Future Analysis property is set to , the file, file.full, is not created and the is not available.
: The option available in the Solution Output property of the Solution Information object.
: The option is not available in the Solution Output property of the Solution Information object. This option is not allowed if the Future Analysis property of the Analysis Data Management category is set to .
General Miscellaneous. Used to access element miscellaneous records via SMISC/NMISC expressions for user defined results. The default value is .
Note: To ensure that Membrane and Bending Stress results are not under-defined, set this option to Yes.
Store Modal Results. Available for Modal analyses only. This field is displayed only when Stress and/or Strain are set to Yes, implying that stress and strain results are to be expanded and saved to file.mode, in addition to displacement results (mode shapes). Depending on the downstream linked analysis, you may want to save these modal stress and/or modal strain results, which are linearly superimposed to get the stress and/or strain results of the downstream linked analysis. This reduces computation time significantly in the downstream linked analysis because no modal stress and/or modal strain results are expanded again. The following options are available:
Program Controlled (default setting): Let the program choose whether or not the modal results are saved for possible downstream analysis.
No: Stress and strain results are not saved to file.mode for later use in the downstream linked analyses. This option is recommended for the linked Harmonic Response analysis due to load generation, which requires that stresses and/or strains are expanded again as a result of the addition of elemental loads in the linked Harmonic Response analysis.
For Future Analysis: Stress and strain results are saved to file.mode for later use in the downstream linked analyses. This option is recommended for a linked random vibration analysis. Choosing this option improves the performance and efficiency of the linked random vibration analysis because, with no load, there is no need for stress and strain expansion.
MSUP Harmonic analyses (Linked and Standalone). This field is displayed only when Stress, and/or the Strain, and/or the Calculate Reactions properties are set to Yes, implying that stress, strain, and reaction results are to be expanded and saved to file.mode after the load generation. Depending on the number of modes and number of frequency steps, you may want to save these modal stresses and/or strains after the load generation, which can be linearly superimposed to obtain harmonic stresses and/or strains at each frequency step. The following options are available for this property:
(default setting): Let the program choose whether or not the stress, strain, and reaction results are expanded and saved for possible downstream analysis. When the option is chosen, the read-only Details view property Expansion is displayed. This indicates whether the stress, strain and reaction results are expanded from the modal solution or harmonic solution.
: Stress, strain, and reaction results are not expanded nor saved to file.mode after the load generation in the MSUP Harmonic system (linked and standalone). This option is recommended when the number of frequency steps is far less than the number of modes. In this option, the stress, strain, and/or reaction results are expanded from harmonic displacement at each frequency step. In this case, stress, strain, and/or reaction expansion is performed as many times as the number of frequency steps.
: Stress, strain, and reaction results are expanded and saved to file.mode after the load generation in the MSUP Harmonic system (linked and standalone). This option is recommended when the number of frequency steps is far more than the number of modes. In this option, the stress, strain, and/or reaction results are calculated by linearly combining the modal stresses, modal strains, and/or modal reactions expanded after the load generation. In this case, stress, strain, and/or reaction expansion are performed as many times as the number of modes.
Refer to Recommended Settings for Modal and Linked Analysis Systems for further details.
Linked Transient analyses. This field is displayed only when the Stress, and/or the Strain, and/or the Calculate Reactions properties are set to Yes, implying that stress, strain and reaction results are to be expanded and saved to file.mode after the load generation. Depending on the number of modes and total number of sub steps/ time steps, you may want to save these modal stresses and/or strains after the load generation, which can be linearly superimposed to obtain transient stresses and/or strains at each time step. The following options are available for this property:
(default setting): Let the program choose whether or not the stress and strain results are expanded and saved for possible downstream analysis. When the option is chosen, the read-only Details view property Expansion is displayed. This indicates whether the stress and strain results are expanded from modal solution or transient solution.
: Stress and strain results are not expanded nor saved to file.mode after the load generation in the linked transient analysis system. This option is recommended when the number of time steps accumulated over all the load steps is far less than the number of modes. In this option, the stress and/or strain results are expanded from transient displacement at each time step. In this case, stress and/or strain expansion is performed as many times as the number of time steps.
: Stress and strain results are expanded and saved to file.mode after the load generation in the linked transient system. This option is recommended when the number of time steps accumulated over all the load steps is far more than the number of modes. In this option, the stress and/or strain results are calculated by linearly combining the modal stresses and/or modal strains expanded after the load generation. In this case, stress and/or strain expansion are performed as many times as the number of modes.
Refer to Recommended Settings for Modal and Linked Analysis Systems for further details.
If you are using the Samcef solver interface for your analysis, the SAI
Command setting can be used to control the SAI codes written in the solver
input file. When this setting is set to Program Controlled, the SAI
codes are taken from the configuration file, stored in
ANSYS_INSTALL_DIR\v182\AISOL\WBAddins\SamcefAddin\SamcefArchiveSettings.xml.
If this option is set to Manual, the text field SAI
Command List option is shown, and the SAI ARCH codes written to the input
file are taken from this field instead of the configuration file. For more information
about the configuration file, see The Samcef Result Storage Configuration File.
If you are using the ABAQUS solver interface, there are several options to control the output of Elements and Nodes from that solver:
The Nodal/Elemental/Contact/Radiation Outputs field
controls result codes sent to the solver. When set to Program
Controlled, the codes are provided from the configuration file
ANSYS_INSTALL_DIR\v182\AISOL\WBAddins\AbaqusAddin\AbaqusArchiveSettings.xml.
When set to Manual, the text field Outputs
List appears and allows you manually set the result codes. When set to
All, the solver stores all results. Note that only the fields
valid for the type of analysis you are performing are shown. For more information
about the configuration file, see The ABAQUS Result Storage Configuration File.
The Output Storage/Output Storage Value fields define the type of result storage.
For a modal analysis, the Mode Selection field allows you to select all modes for output, or define a subset of modes manually.
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.
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:
Store Results At. Based on the analysis type, specify this time to be All Time Points or All Iterations (default setting), Last Time Point or Last Iteration, Equally Spaced Points or Specified Recurrence Rate.
Value. Displayed only if Store Results At is set to Equally Spaced Points or Specified Recurrence Rate.
The following table provides a summary of recommended settings for Store Modal Results and Expand Results From based on the analysis type.
| Analysis Type | Recommended Store Modal Results Settings | Recommended 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 . | Program controlled. |
| Static Structural with downstream linked Topology Optimization |
For Future Analysis The Nodal Forces property is set to . | 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
The Mechanical application cannot post process split result files produced by the ANSYS solver. Try either of the following workarounds should this be an issue:
Use Output Controls to limit the result file size. Also, the size can more fully be controlled (if needed) by inserting a Commands object for the OUTRES command.
Increase the threshold for the files to be split by inserting a Commands object for the /CONFIG,FSPLIT command.