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. These properties enable you to control the size of the results file which can be beneficial when performing a large analysis.
The following Output Controls properties 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.
Output Selection: Use this property to store results on specific geometry or mesh selections to reduce result file size. Only supported for elemental-based results that have an associated Output Control property, such as Stress or Nodal Forces, whose property is set to . Options include (default) and . When you select , a property displays. Use this property to specify one or more geometry- or meshed-based Named Selections. During the solution process, the application only writes element nodal result quantities to the result file for the geometry or mesh associated with these named selections.
- Notes
This property is only supported for analyses that have the Solver Type property of the Environment object set to .
You should include probe and contact results in the scoping of the named selection for proper evaluation.
- Limitations
Note the following limitations associated with this property:
The application does not send Named Selections specified by this property to the solver if you set the:
Send As property to for element face-based Named Selections.
Send to Solver property is set to . The default setting is .
If you import loads from an upstream system that specifies Named Selections using this property, the application imports only the load data associated with the entities scoped to these Named Selections.
For a result with the Scoping Method to , only the exposed element faces of the Named Selection present contour colors. Exposed faces are not shared by multiple elements. Use the setting for the Scoping Method property to display contour colors on the whole elements.
If your analysis includes Condensed Part objects, you cannot specify its scoping with a Named Selection used by this property. The application will ignore the Named Selection during the solution process.
If your analysis includes a Symmetry object, the application will ignore the Named Selection during the solution process.
The Fatigue Tool is not affected by this feature.
If your analysis includes a Nonlinear Adaptive Region, Geometry Based Adaptivity, or a SMART Crack Growth object, the application will not produce results for the selected named selections if remeshing occurs on them.
Stress. Writes element nodal stresses to the results file. The default value is . Available for Coupled Field analyses, Static Structural, Transient Structural, Modal, and Eigenvalue Buckling analysis types.
Note: There are two options to obtain surface stress results. You can use the Surface Coating feature to accurately evaluate surface stresses. Or you can use a Command (APDL) object. To properly define this object, see the Mechanical APDL Element Reference for key options to activate surface solution results on eligible elements as well as the Solution Output topic for the steps to obtain the surface solution as tabular data.
Back Stress: Writes element back stresses to the result file. Options include and (default). Available for material models that have kinematic hardening. See the Mechanical APDL OUTRES command section for supported models.
Strain. Writes element elastic strains to the results file. The default value is . Available for Coupled Field analyses, Static Structural, Transient Structural, Modal, and Eigenvalue Buckling analysis types.
Contact Data: Writes element contact data to the result file. Options include (default) and . Available for an Additive Manufacturing Process Simulation, Coupled Field analyses, Static Structural, Transient Structural, Modal, Harmonic Response, Eigenvalue Buckling, Steady-State thermal, Transient Thermal, Electric, and Thermal-Electric analyses.
Note: For an Additive Manufacturing Process Simulation, the default setting is in order to reduce the size of the result file.
Nonlinear Data: Writes element nonlinear data to the result file. Options include and (default). Available for Coupled Field Static, Coupled Field Transient, Static Structural, and Transient Structural analyses. See the User Defined Results for Nonlinear Analyses topic in the User Defined Results for the Mechanical APDL Solver section for the specific Items supported by the command. These items are accessed through the Solution Quantities and Result Summary page of the Worksheet following the solution process.
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.
Euler Angles. Requests Euler Angle result values be written to the result file. Available for all analysis types except Response Spectrum, Random Vibration, and Structural Optimization analyses. The default is .
Note:For a Modal, Eigenvalue Buckling, and an Additive Manufacturing Process Simulation, the default setting is in order to reduce the size of the result file.
The application may skip the evaluation of Euler Angles if the element coordinate system is aligned with Global Coordinate System.
Important: Some result types, such as stress and/or strain results, may require Euler angle result data to properly display a result in the desired coordinate system. When the Euler Angle property is set to , the result file may still contain the Euler angle results if any of the elemental results are set to . However, if the Euler Angle property is set to and all the elemental result outputs are also set to , the application produces an error message and no result contours display for the elements in need of Euler angles.
Volume and Energy. Writes summed volume and energy values to the result file: data that is essential for results such as Volume Probes, Energy Probes, Structural Error, etc. Available for all analysis types except Response Spectrum, Random Vibration, and Structural Optimization analyses. The default is .
Note: For a Modal, Eigenvalue Buckling, and an Additive Manufacturing Process Simulation, the default setting is in order to reduce the size of the result file.
Calculate Reactions. Turn On for Nodal Forces on constraints. Available for Coupled Field Harmonic, Coupled Field Modal, Modal, and Transient (when linked to a upstream Modal system) 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.
Note: During a MSUP Transient analysis, the Force Reaction probe contains only the static contribution if you set the Calculate Velocity and Acceleration property to . Review the TRNOPT command in the Mechanical APDL Command Reference for more information.
Calculate Thermal Flux. Available for an Additive Manufacturing Process Simulation, Coupled Field Static, Coupled Field Transient, Steady-State Thermal, and Transient Thermal analysis types.
Note: For an Additive Manufacturing Process Simulation, the default setting is in order to reduce the size of the result file.
Heat Generation Rate: Writes element heat generation rate to the result file. Options include (default) and . Available for Coupled Field analyses, Electric, and Thermal-Electric analyses.
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 (for example, 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 Coupled Field Static, Coupled Field Transient, Static, and Transient Structural analysis types. Not Available when linked to a Modal analysis.
Element Current Density: Writes element current densities to the result file. Options include and (default). Available for Coupled Field Static, Coupled Field Transient, Electric, Thermal-Electric, and Magnetostatic analyses.
Electromagnetic Nodal Forces: Writes element electromagnetic nodal forces to the result file. Options include and (default). Available for Magnetostatic analyses.
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. Options include /. The default value is .
Note: To ensure that Membrane and Bending Stress results are not under-defined, set this option to Yes.
- Acoustics Analyses Only
Setting this property to during an Acoustics analysis causes the application to also display the Value sub-property. The Value property enables you to select the bodies of your model for which the application sends element-based miscellaneous solution data to the output file. Options include:
: The action of this property depends upon the acoustics analysis type.
- Harmonic Acoustics
This option issues miscellaneous data for all acoustic bodies if your analysis includes a Far-Field Radiation Surface (that you manually defined or that the application automatically generated), a Free Surface boundary condition, a Diffuse Sound Field excitation, or an acoustic Port.
- Modal Acoustics
This option issues miscellaneous data for all acoustic bodies if your analysis includes a Free Surface boundary condition.
: This option generates miscellaneous data for all bodies.
: This option generates miscellaneous data for all acoustic bodies.
: This option generates miscellaneous data for all structural bodies.
Note: Setting the General Miscellaneous property to invalidates all Free Surface boundary conditions as well as all Far-field results.
Store Modal Results (Modal analyses only). This field is only displayed when one of the element-based Output Controls is set to , such as Stress, Strain, etc. This implies that element-based results must 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: Element-based results are not saved to file.mode for later use in the downstream analyses. This option is recommended for a 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: Element-based results are saved to file.mode for later use in the downstream linked analyses. This option is recommended for linked Random Vibration and Response Spectrum analyses. For these analysis types, the application does not need to solve elemental results, therefore, this setting improves performance and efficiency.
MSUP Harmonic Analyses (Linked and Standalone). For this analysis type, the Expand Results From property displays only when one or more of the following results are set to :
Stress Strain Calculate Reactions Euler Angles Volume and Energy Contact Data Activating one or more of these properties implies that one or more of the above 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. However, if the Options > Cluster Results property is set to and you specify a high number of Modes, the solution is expanded from Harmonic Response analysis. If a lower number of Modes is specified, the solution is expanded from the Modal analysis.
: 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.
Note: For a MSUP Harmonic Response analysis linked to an upstream Modal Analysis that (1), includes a defined Constant Damping Coefficient in the Engineering Data Workspace and (2), the Eqv. Damping Ratio From Modal property set to (Analysis Settings > Damping Controls), you cannot expand results from the Harmonic solution unless the elemental results are expanded during the upstream modal solution. You must set the Stress, Strain, and/or Calculate Reactions properties to in upstream Modal analysis to expand the elemental results. See the MXPAND section of the Mechanical APDL Command Reference for more information.
: 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.
Important: For MSUP Harmonic Response analysis, if you 1) scope a Force Reaction probe to a Remote Point or a Remote Boundary Condition and 2) set the Expand Results From property of the Harmonic Response analysis to either:
Or...
with the Expansion property set to Modal Solution.
Then the Force Reaction probe includes the static contribution only. For more information, see the Reaction Forces topic in the Mechanical APDL Theory Reference.
Refer to Recommended Settings for Modal and Linked Analysis Systems for further details.
Linked Transient Analyses. For this analysis type, the Expand Results From property displays only when one or more of the following properties are set to :
Stress Strain Calculate Reactions Euler Angles Volume and Energy Contact Data Activating one or more of these properties implies that one or more of the above 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.
Note: For a Transient Structural analysis linked to an upstream Modal Analysis that (1), includes a defined Constant Damping Coefficient in the Engineering Data Workspace and (2), the Eqv. Damping Ratio From Modal property set to (Analysis Settings > Damping Controls), you cannot expand from the Transient solution unless the elemental results are expanded during the upstream modal solution. You must set the Stress, Strain, and/or Calculate Reactions properties to in upstream Modal analysis to expand the elemental results.
: 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.
Important: For MSUP Transient analysis, if you 1) scope a Force Reaction probe to a Remote Point or a Remote Boundary Condition and 2) set the Expand Results From property of the Harmonic Response analysis to either:
Or...
with the Expansion property set to Modal Solution.
Then the Force Reaction probe includes the static contribution only. For more information, see the Reaction Forces topic in the Mechanical APDL Theory Reference.
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\v242\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\v242\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.
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 Structural 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. For Additive Manufacturing simulations, options include All Layers, Last Heating and Cooling Steps, and Every N Layers.
Value. Displayed only if Store Results At is set to Equally Spaced Points or Specified Recurrence Rate.
Result File Compression: This property enables you to generate a compressed result file. Options include (default), , . The and settings instruct the application to compress the file.
Export Layer End Temperature. No (default) or Yes. This setting controls whether the temperature of a layer just before a new layer is applied is written out to an AMResults.txt file. Available for Additive Manufacturing thermal analyses only.
Export Recoater Interference. No (default) or Yes. This setting controls whether the z-deformation of a layer just before a new layer is applied is written out to an AMResults.txt file. Available for Additive Manufacturing structural analyses only.
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 Type | Recommended Store Modal Results Settings | Recommended Expand Results From Settings |
|---|---|---|
| Modal with no downstream 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[a] 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 linked to downstream 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 linked to downstream 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 linked to downstream Structural Optimization analysis |
For Future Analysis The Nodal Forces and the General Miscellaneous properties are set to . | Program Controlled. |
| Static Structural linked to downstream Structural Optimization analysis |
For Future Analysis The Nodal Forces property is set to . | Program Controlled. |
| Modal linked to downstream Transient analysis |
No[a] 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. |
[a] Review the Requirements and Limitations for Modal and Linked MSUP Analysis Systems shown below.
- Requirements and Limitations for Modal and Linked MSUP Analysis Systems
If you have an MSUP analysis, either Harmonic Response or Transient, linked to an upstream Modal system, the Modal analysis does not respect the Expand Results From property setting when:
Only Direct FE loads, Remote Force, or Moment are scoped to global remote points.
The analysis includes a Commands (APDL) object.
No Damping Ratio is specified.
If the material damping is specified using the Eqv. Damping Ratio From Modal property (set to ) and at least one of the elemental-based Output Controls (Stress, Strain, etc.) is also set to in the linked Modal analysis.
Instead, it will be driven by the Store Modal Results property (of the Modal system):
Setting this property to , the Expand Results From property of the MSUP Harmonic Response or Transient analysis is ignored, even if set to . The results would be as if the or option had been set. Given this internal specification, you do not receive the results you expected.
Setting the property to , the Expand Results From property of the MSUP Harmonic Response or Transient analysis is ignored. The results would be as if the option had been set. In this case, be sure that you request the same results from the Output Controls settings for both the Modal and downstream MSUP analyses. Given this internal specification, you do not receive the results you expected.
The scenarios are summarized in the following table.
Store Modal Results Property Setting Expand Result From Property Setting Actual Expanded Results No Expand from Modal Expanded from Harmonic/Transient No Expand from Harmonic/Transient Expanded from Harmonic/Transient For Future Analysis Expand from Modal Expanded from Modal For Future Analysis Expand from Harmonic/Transient Expanded from Modal - Limitations When Using the Mechanical APDL Solver
The Mechanical application cannot post process split result files produced by the Mechanical APDL 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.