Using the Options dialog, you can control various behaviors and default functions of the application to better suit your uses. This feature essentially enables you to establish preferences for application behaviors and property settings.
To open and make changes to Options settings:
Select > . A dialog box titled Options displays. Groupings associated with default behaviors for the application display under the Mechanical heading. These groups are referred to as categories. Within each category are various properties that you can change the settings for. For example, and as illustrated below, the Connections category is highlighted by default. Here you can see that you can specify a value for the Face Overlap Tolerance from the default of zero (0). These types of customizations can be very beneficial.

Select a desired category. Each category has associated properties.
Change any of the property settings by clicking directly in the field. You will first see a visual indication for the kind of interaction required in the field (examples are drop-down menus, secondary dialog boxes, direct text entries).
Click .
Important: Option settings within a particular language are independent of option settings in another language. If you change any options from their default settings, then start a new Workbench session in a different language, the changes you made in the original language session are not reflected in the new session. You are advised to make the same option changes in the new language session.
Select a link below to jump to the topic concerned with the desired application preference:
| Connections |
| Convergence |
| Import |
| Export |
| Fatigue |
| Frequency |
| Geometry |
| Meshing |
| Graphics |
| Miscellaneous |
| Report |
| Analysis Settings and Solution |
| Results |
| Visibility |
| Wizard |
The Auto Detection category enables you to change the default values in the Details view for the following:
Note: The auto contact detection on geometry attach can be turned on/off from the Workbench Options dialog box for the Mechanical application. See the Mechanical part of the Setting ANSYS Workbench Options section of the Help.
Tolerance: Sets the default for the contact detection slider; that is, the relative distance to search for contact between parts. The higher the number, the tighter the tolerance. In general, creating contacts at a tolerance of 100 finds fewer contact surfaces than at 0. The default is . The range is from -100 to +100.
Face Overlap Tolerance: Sets the default tolerance for overlap of faces in contact; that is, the minimum percentage of overlap at which a contact pair is created for two overlapping faces. For example, if Face Overlap Tolerance is set to 25, a contact pair is created for each pair of faces for which at least 25% of one face overlaps the other. This setting enables the software to obtain more precise contact pairs during automatic contact generation based on a tolerance that is appropriate for your simulation type. The default is 0, which means overlap checks are turned off. The range is from 0 to 100.
Note: The Face Overlap Tolerance value and the Tolerance value are evaluated together to determine which faces are considered to be in contact.
Face/Face: Sets the default preference1 for automatic contact detection between faces of different parts. The choices are or . The default is .
Cylindrical Faces: Set the default for separating flat surfaces from cylindrical faces for face/face contact. Options include (default), , and .
Face/Edge: Sets the default preference1 for automatic contact detection between faces and edges of different parts. The choices are:
(default)
Edge Overlap Tolerance: Sets the default tolerance for overlap of an edge and a face in contact; that is, the minimum percentage of overlap at which a contact pair is created for an edge and a face that overlap. For example, if Edge Overlap Tolerance is set to 25, a contact pair is created for an edge and a face when at least 25% of the edge overlaps the face. This setting enables the software to obtain more precise contact pairs during automatic contact generation based on a tolerance that is appropriate for your simulation type. The default is 0, which means overlap checks are turned off. The range is from 0 to 100.
Edge/Edge (3D): Sets the default preference1 for automatic contact detection between edges of different parts in a three dimensional model. The choices are or . The default is .
Edge/Edge (2D): Sets the default preference1 for automatic contact detection between edges of different parts in a two dimensional model. The choices are or . The default is .
Priority: Sets the default preference1 for the types of contact interaction priority between a given set of parts. The choices are:
(default)
Revolute Joints: Sets the default preference for automatic joint creation of revolute joints. The choices are Yes and No. The default is Yes.
Fixed Joints: Sets the default preference for automatic joint creation of fixed joints. The choices are Yes and No. The default is Yes.
1 Unless changed here in the Options dialog box, the preference remains persistent when starting any Workbench project.
The Transparency category includes the following exclusive controls for this category. There are no counterpart settings in the Details view.
Parts With Contact: Sets transparency of parts in selected contact region so the parts are highlighted. The default is 0.8. The range is from 0 to 1.
Parts Without Contact: Sets transparency of parts in non-selected contact regions so the parts are not highlighted. The default is 0.1. The range is from 0 to 1.
The Default category enables you to change the default values in the Details view for the following:
Type: Sets the definition type of contact. The choices are:
(default)
Behavior: Sets the contact pair. The choices are:
(default)
Formulation: Sets the type of contact formulation method. The choices are:
(default)
Update Stiffness: Enables an automatic contact stiffness update by the program. The choices are:
(default)
Shell Thickness Effect: This setting enables you to automatically include the thickness of surface bodies during contact calculations. The default setting is No.
Auto Rename Connections: Automatically renames joint, spring, contact region, and joint condition objects when Type or Scoping are changed. The choices are Yes and No. The default is Yes.
The Convergence category enables you to change the default values in the Details view for the following:
Target Change: Change of result from one adapted solution to the next. The default is 20. The range is from 0 to 100.
Allowable Change: This should be set if the criteria is the max or min of the result. The default is Max.
The Solution category enables you to change the default values in the Details view for the property. This property enables you to change the number of refinement loops the application performs. The default is . The range is from to . When performing an out of process solution asynchronously, wherein the solve may finalize during another Workbench session, the application performs only one maximum refinement loop. As necessary, you must manually perform additional loops. To solve with a single user action, solve synchronously.
The Import category enables you to specify preferences for when you import data into Mechanical. Currently, these preferences are for importing delamination interfaces from the ANSYS Composite PrepPost (ACP) application.
Create Delamination Objects: This option controls the automatic creation of Interface Delamination objects in Mechanical when importing layered section data from ACP. When Interface layers are specified in ACP, Interface Delamination objects corresponding to Interface Layers are automatically inserted into the Mechanical Tree Outline under the Fracture object. The default setting is .
Delete Invalid Objects: This option controls the deletion of Invalid Interface Delamination objects scoped to Interface Layers from ACP. When an Interface Layer specified in ACP is deleted, the corresponding Interface Delamination object is deleted in Mechanical when the project is refreshed. The default setting is . This default setting suppresses invalid objects instead of automatically deleting them.
The Text File Export category provides the following exclusive settings. There are no counterpart settings in the Details view.
File Encoding: select either (default) or as the encoding to use for exporting data.
Automatically Open Excel: Excel will automatically open with exported data. The default is .
Include Node Numbers: Node numbers will be included in exported file. The default is .
Include Node Location: Node location can be included in exported file. The default is .
Show Tensor Components: Options include and (default). For the default setting , the export data contains the principal stresses and strains (1, 2, and 3) as well as the three Euler angles. The export data for the setting contains raw components of stress and strain (X, Y, Z, XY, YZ, XZ).
The STL Export category provides the setting Export Format. This property sets the default for how STL files are exported, using either (default) or format.
The AVZ Viewer Option category provides the property Open AVZ Viewer. When this property is set to , the application automatically opens the ANSYS Viewer (after you have saved the file) when you are exporting a result object using the contextual menu option . When set to , the application simply prompts you to save the AVZ file. This feature applies to result objects only.
The General category enables you to change the default values in the Details view for the following:
Design Life: Number of cycles that indicate the design life for use in fatigue calculations. The default is 1e9.
Analysis Type: The default fatigue method for handling mean stress effects. The choices are:
(default)
The Goodman, Soderberg, and Gerber options use static material properties along with S-N data to account for any mean stress while Mean-Stress Curves use experimental fatigue data to account for mean stress.
The Cycle Counting category enables you to change the default values in the Details view for the following:
: The bin size used for rainflow cycle counting. A value of 32 means to use a rainflow matrix of size 32 X 32. The default is 32. The range is from 10 to 200.
The Sensitivity category enables you to change the default values in the Details view for the following:
Lower Variation: The default value for the percentage of the lower bound that the base loading will be varied for the sensitivity analysis. The default is 50.
Upper Variation: The default value for the percentage of the upper bound that the base loading will be varied for the sensitivity analysis. The default is 150.
Number of Fill Points: The default number of points plotted on the sensitivity curve. The default is 25. The range is from 10 to 100.
Sensitivity For: The default fatigue result type for which sensitivity is found. The choices are:
Life (default)
Damage
Factor of Safety
The Modal category enables you to change the Modal Analysis default values in the Details view for the following:
Max Number of Modes: The number of modes that a newly created frequency branch will contain. The default is 6. The range is from 1 to 200.
Limit Search to Range: You can specify if a frequency search range should be considered in computing frequencies. The default is No.
Min Range (Hz): Lower limit of the search range. The default is value is 0.01 for Modal Acoustic analyses and 0.0 all other analysis types.
Max Range (Hz): Upper limit of the search range. The default is value is 100000000.
Cyclic Phase Number of Steps: The number of intervals to divide the cyclic phase range (0 - 360 degrees) for frequency couplet results in cyclic modal analyses.
The Eigenvalue Buckling category enables you to change the Eigenvalue Buckling Analysis default values in the Details view for the Max Modes to Find property. This property defines the number of buckling load factors and corresponding buckling mode shapes. The default value is 2.
The Harmonic category enables you to change the default setting in the Details view for the Frequency Spacing property. The options include:
(default)
The Geometry category enables you to change the default values in the Details view for the following:
Beam Cross Section (For Solver): define the default setting to send user-defined cross-sections, to the Mechanical APDL solver, as either a (default) cross-section or as a section.
Nonlinear Material Effects: Indicates if nonlinear material effects should be included (Yes), or ignored (No). The default is .
Thermal Strain Calculation: Indicates if thermal strain calculations should be included (Yes), or ignored (No). The default is .
Note: This setting applies only to newly attached models, not to existing models.
The Material category provides the setting Prompt for Model Refresh on Material Edit. This setting relates to the material Assignment property. If you choose to edit a material or create/import a new material via this property, the application displays a message (illustrated below) reminding you to refresh the Model cell in the Workbench Project Schematic. The default setting is . The message in Mechanical provides you with the option to not show the message again. This option is in addition to this method of changing this setting to .

The Meshing category enables you to change the value of Default Physics Preference. The physics preference that you choose here will be the default for all Mechanical systems, regardless of whether they are analysis systems or component systems. The choices are:
(default)
Note: The default physics preference that you can set in the Meshing application's Options dialog box has no effect on the default that is set for Mechanical systems.
The Default Graphics Options category enables you to change the default values in the Details view for the following:
Reset Views on Geometry Refresh: Select whether geometry refreshes will reset the graphical view in Mechanical. The default setting is .
Max Number of Annotations to Show: A slider that specifies the number of annotations that are shown in the legend of the Geometry window. The range is adjustable from 0 to 50. The default is .
Show Min Annotation: Indicates if Min annotation will be displayed by default (for new databases). The default setting is .
Show Max Annotation: Indicates if Max annotation will be displayed by default (for new databases). The default setting is .
Contour Option: Selects default contour option. The options include:
(default)
Flat Contour Tolerance: Flat contours (no variation in color) display if the minimum and maximum results values are equal. The comparison of the minimum and maximum values is made using scientific notation with the number of significant digits to the right of the decimal point as specified with the flat contour tolerance setting ( to ). Increasing this tolerance enables you to display contours for an otherwise too narrow range of values. Decreasing this tolerance prevents insignificant range variations from being contoured. This setting has a default value of .
Edge Option: Selects default edge option. The choices are:
(default)
Highlight Selection: Indicates default face selection. The choices are:
(default)
Number of Circular Cross Section Divisions: Indicates the number of divisions to be used for viewing line body cross sections for circular and circular tube cross sections. The range is adjustable from 6 to 360. The default is 16.
Mesh Visibility: Indicates if mesh is automatically displayed when the Mesh object is selected in the Tree Outline, or if it’s only displayed when you select the Show Mesh button. The default is Automatic.
FE Annotation Color: This option enables you to change the default coloring for FE related annotations (FE-based Named Selections and/or Objects scoped to Nodes or Elements). It also changes the color of the elements displayed for an Analysis Ply object.
Model Rotation Center: This option enables you to change how the rotation feature behaves. Options include:
(default): Select a location on the model to be the center of rotation.
: Select a location on the model to be the center of rotation. Rotation is available immediately - no additional mouse selections ("clicks") are required.
Max Number of Labels to Shown in Legend: A slider that specifies the number of annotations that are shown in the legend of the Graph window when you are using Charts. The range is adjustable from 0 to 50. The default is 10.
Shell Expansion Edge Angle: This option enables you to change the setting for the angle used to determine whether adjacent element normals are averaged. This is applicable when shell thickness is being applied to the mesh to represent the actual thickness. The range is adjustable from 0 to 180. The default is 180.
Line Body Thickness: This option enables you to change how line bodies are displayed in the Geometry window. Selections include (default) and .
The Image Export category defines the resolution, image content, background characteristics, and font size contained on the image when you save it as a file using the Image to File option on the New Figure or Image menu on the Standard Toolbar, or when you create a Figure, or when you prepare a Print Preview of an object or a Report Preview. It includes the following properties:
Graphics Resolution: Defines default resolution setting. Options include:
(default and only Linux option)
Note: The ANSYS logo does not scale at higher resolution settings.
Capture: Defines whether the legend is included in the image. Options include:
(default)
Background: Defines the background coloring. Options include:
(default): ANSYS Mechanical setting or user-defined background color.
Show Preferences Dialog: Yes (default) or No. This option determines whether a dialog box automatically displays when you select the Image to File option. The dialog box contains all of the above options. If disabled using this option, the application saves the most recent settings that you have used.
Font Magnification Factor: This setting changes the font
size of the textual content contained in the legend. The magnification range for
the font size is 0.5 to 1.5. If you
enter a value less than or greater than this range, the application will default
to the corresponding minimum (0.5) or maximum
(1.5) value. The default value is
1. This setting also scales the contour color
band.
The UI Controls category contains the property Details View Combo Boxes. This property enables you to change the default setting for the ability to search drop-down lists in the Details view. The options include: (default) and .
The Miscellaneous category enables you to change the default values in the Details view for the following:
Load Orientation Type: Specifies the orientation input method for certain loads. This input appears in the Define By option in the Details view of the load, under Definition.
Vector (default)
Component
Report Performance Diagnostics in Message: Turn on messaging that reports the time it takes for certain processes to execute, such as the time it takes for contact detection, mesh generation, writing the input file, solution, etc. Options include and (default).
Message Coloring: Set whether to have the application highlight objects in the tree that are experiencing an issue. The objects as well as the corresponding message in the Messages window can be highlighted or you can select to highlight only Message window content. The available options include (default), , and .
Note: You need to close and then reopen Mechanical in order for changes to this preference to take effect.
The Image category includes the following exclusive controls for this category. There are no counterpart settings in the Details view.
Image Transfer Type: Defines the type of image file created when you send an image to Microsoft Word or PowerPoint, or when you select Print Preview. The choices are:
(default)
The Post Processing (MAPDL Only) category includes the following controls for results files written by the Mechanical APDL solver:
Result File Caching: By holding substantial portions of a file in memory, caching reduces the amount of I/O associated with result file reading. The cache can, however, reduce memory that would otherwise be used for other solutions. The choices are:
System Controlled (default): The operating system determines whether or not the result file is cached for reading.
Off: There is no caching during the reading of the result file.
Program Controlled: The Mechanical application determines whether or not the result file is cached for reading.
Note: You need to close and then reopen Mechanical in order for changes to this preference to take effect.
The Save Options category includes the following controls for this category.
Save Project Before Solution: Sets the Yes / No default for the Save Project Before Solution setting located in the Project Details panel. Although you can set the default here, the solver respects the latest Save Project Before Solution setting in the Details panel. The default for this option is No. Selecting Yes saves the entire project immediately before solving (after any required meshing). If the project had never been previously saved, you can now select a location to save a new file.
Save Project After Solution: Sets the Yes / No default for the Save Project After Solution setting in the Project Details panel. The default for this option is No Selecting Yes Saves the project immediately after solving but before postprocessing. If the project had never been previously saved, nothing will be saved.
Note: The save options you specify on the Project Details panel override the options specified in the Options dialog box and will be used for the current project.
The Figure Dimensions (in Pixels) category includes the following controls that allow you to make changes to the resolution of the report for printing purposes.
Chart Width - Default value equals pixels.
Chart Height - Default value equals pixels.
Graphics Width - Default value equals pixels.
Graphics Height - Default value equals pixels.
Graphics Resolution - Resolution values include:
The Customization category includes the following controls:
Maximum Number of Table Columns: (default = columns) Changes the number of columns used when a table is created.
Merge Identical Table Cells: merges cells that contain identical values. The default value is .
Omit Part and Joint Coordinate System Tables: chooses whether to include or exclude Coordinate System data within the report. This data can sometimes be cumbersome. The default value is .
Include Figures: specifies whether to include Figure objects as pictures in the report. You may not want to include figures in the report when large solved models or models with a mesh that includes many nodes and elements are involved. In these cases, figure generation can be slow, which could significantly slow down report generation. The default value is .
Note: This option applies only to Figure objects as pictures. Graph pictures, Engineering Data graphs, and result graphs (such as phase response in a harmonic analysis) are not affected and will appear regardless of this option setting.
Custom Report Generator Folder: reports can be run outside of the Workbench installation directory by copying the Workbench folder to a new location. Specify the new folder location in this field. See the Customize Report Content section for more information.
The Solver Controls category enables you to change the default values in the Details view for the following:
Solver Type: Specifies which ANSYS solver will be used. The choices are:
(default)
Use Weak Springs: specifies whether weak springs are added to the model. The setting automatically enables weak springs to be added if an unconstrained model is detected, if unstable contact exists, or if compression only supports are active. The choices include:
(default)
Solver Pivot Checking: Sets the default for all new analyses created. Options include:
(default): enables the solver to determine the response.
: Instructs the solver to continue upon detection of the condition and attempt the solution.
: Instructs the solver to stop upon detection of the condition and issue an error message.
: Pivot checking is not performed.
The Solver Control (Eigenvalue Buckling) category provides the Include Negative Load Multiplier property. Options include (default), , and . This option enables you to evaluate either negative and positive load multipliers or only positive load multipliers. The setting evaluates positive load multipliers given the load directions. The setting evaluates positive load multipliers given the load directions as well as the negative load multipliers by flipping the load directions.
The Output Controls (Static and Transient) category enables you to change the default values in the Details view for the following:
Stress (Default setting = Yes)
Strain (Default setting = Yes)
Nodal Forces (Default setting = No)
Contact Miscellaneous (Default setting = No)
General Miscellaneous (Default setting = No)
Calculate Reactions (Default setting = Yes)
Calculate Thermal Flux (Default setting = Yes)
The Output Controls (Modal) category enables you to change the default value in the Details for the following:
Stress: Writes stress results to the file, file.mode. Options include (default) and .
Strain: Writes strain results to the file, file.mode. Options include (default) and .
Store Modal Results: Options include (default), , or .
The Options (Random Vibration) category enables you to change the default value in the Details view for the following:
Exclude Insignificant Modes: When set to , this property enables you to exclude modes for the mode combination based on the entry of the Mode Significance Level property. The default setting is .
Mode Significance Level: This property defines
the threshold for the numbers of modes for mode combination. The default setting
is 0 (all modes selected). Supported entries are between
0.0 and 1. Displayed only when
Exclude Insignificant Modes is set to
.
The Output Controls (Random Vibration) category enables you to change the default value in the Details view for the following:
Keep Modal Results: include or remove modal results from the result file of Random Vibration analysis. The default setting is .
Calculate Velocity: Write Velocity results to the results file. The default setting is .
Calculate Acceleration: Write Acceleration results to the results file. The default setting is .
The Restart Controls category enables you to change the default value in the Details view for the following:
Generate Restart Points: (default setting) automatically generates restart points. Additional options include , that provides user-defined settings, and , which restricts the creation of new restart points.
Retain Files After Full Solve: when restart points are requested, the necessary restart files are always retained for an incomplete solve due to a convergence failure or user request. However, when the solve completes successfully, you have the option to request to either keep the restart points by setting this field to Yes, or to delete them by setting this field to No.
You can control these settings in the Details view of the Analysis Settings object under Restart Controls, or here under in the Analysis Settings and Solution preferences list. The setting in the Details view overrides the preference setting.
The Solution Information category enables you to change the default value in the Details view for the following:
Refresh Time: specifies how often any of the result tracking items under a Solution Information object get updated while a solution is in progress. The default is 2.5 s.
Activate FE Connection Visibility: specifies the value of the Activate Visibility property. The default setting is .
The Solution Settings category enables you to set the default value in the Details view for the following:
Results Availability: specifies what results to allow under the Solution object in Design Assessment systems when the Solution Selection object allows combinations. The default is Filter Combination Results.
The Analysis Data Management category enables you to specify default settings in the Details view for the following:
Scratch Solver Files Directory: Use this option to specify a unique disk drive that the application will use to process the solution. Using this entry field, you must specify an existing disk location. If the entry is invalid, the application uses the default disk.
Save MAPDL db: Use this option to set the default value in the Details view for the Save MAPDL db control. Selections include (default) or . The setting of the Future Analysis control (see Analysis Data Management Help section) can sometimes require the db file to be written. In this case, the Save MAPDL db control is automatically set to .
The Analysis Data Management (Modal) category enables you to set the default value in the Details view for the Future Analysis property. The options include (default), MSUP Analyses, and Topology Optimization. If this property is set to MSUP Analyses or Topology Optimization, the application creates the files needed for future MSUP analyses or Topology Optimization. If this property is set to , the files are not created in order to improve solution time and reduce file size.
The Analysis Data Management (Static Structural) category enables you to set the default value in the Details view for the Future Analysis property. The options include (default) or . If this property is set to , the application creates the files needed for Topology Optimization. If this property is set to , the files are not created in order to improve solution time and reduce file size.
The Default category of the Results option provides the following controls:
Calculate Time History: Sets the default value for calculation of time history. The default is .
Auto Rename Results: Automatically renames a result when the result Type is changed. The choices are and . The default is .
Average Across Bodies: Change the default setting of the property Average Across Bodies. The options are and . The default setting is .
Prompt Before Deleting Results on Solve: this control enables you to activate a confirmation prompt for the option on the Solution folder’s right-click context menu as well as the child object of the Solution folder (e.g., result objects). The prompt only displays for analyses with existing solution data. The available options include:
(default): You are prompted when you attempt to re-solve a failed solution or for a solution with restart points.
: the confirmation prompt feature is turned off.
: you are always prompted when you select the right-click option.
Note: The F5 hotkey does not support this function.
The Visibility selection and category provides the Part Mesh Statistics setting. This setting enables you to display or hide the Statistics category in the Details view for Body and Part objects.
The Tree Filtering category provides the following controls:
Graphics: (default) or . Setting this option to when the filter is active and set to , causes the tree to automatically filter using that option whenever a body is hidden or shown so that only visible bodies and objects associated with any visible body display.
Expand: or (default). Change the default setting of the Expand on Refresh button on the Filtering toolbar.
The Wizard Options category includes the following exclusive controls for this category. There are no counterpart settings in the Details view.
Default Wizard: This is the URL to the XML wizard definition to use by default when a specific wizard isn't manually chosen or automatically specified by a simulation template. The default is StressWizard.xml.
Flash Callouts: Specifies if callouts will flash when they appear during wizard operation. The default is Yes.
The Skin category includes the following exclusive controls for this category. There are no counterpart settings in the Details view.
Cascading Style Sheet: This is the URL to the skin (CSS file) used to control the appearance of the Mechanical Wizard. The default is Skins/System.css.
The Customization Options category includes the following exclusive controls for this category. There are no counterpart settings in the Details view.
Mechanical Wizard URL: For advanced customization. See Appendix: Workbench Mechanical Wizard Advanced Programming Topics for details.
Enable WDK Tools: Advanced. Enables the Wizard Development Kit. The WDK adds several groups of tools to the Mechanical Wizard. The WDK is intended only for persons interested in creating or modifying wizard definitions. The default is No. See the Appendix: Workbench Mechanical Wizard Advanced Programming Topics for details.
URLs in the Mechanical Wizard follow the same rules as URLs in web pages.
Relative URLs are relative to the location of the Mechanical Wizard URL.
Absolute URLs may access a local file, a UNC path, or use HTTP or FTP.
The Mechanical application stores the configuration information from the Options dialog box in a file called a User Preference File on a per user basis. This file is created the first time you start the Mechanical application. Its default location is:
%APPDATA%\Ansys\v182\%AWP_LOCALE182%\dsPreferences.xml