16.1.17. Analysis Data Management

The properties of the Analysis Data Management category vary based on the type of analysis being performed. Supported analysis types include:

The Analysis Data Management category includes the following properties and options.

Property	Options/Descriptions
Solver Files Directory	This property Indicates the location of the solution files for this analysis. The directory location is automatically determined by the program as detailed in Managing Files. The solution file folder can be displayed using the context Open Solver Files Directory menu option. Open Solver Files Directory Feature This right-click context menu option is available when you have an analysis Environment or a Solution object selected. Once executed, this option opens the operating system's (Windows Only) file manager and displays the directory that contains the solution files for your analysis. The directory path is shown in the Details View. If a solution is in progress, the directory is shown in the Solver Files Directory field. When a solution is in progress, the directory displays in the Scratch Solver Files Directory. For a remote solve, it will open the scratch directory until the results download is complete.
Future Analysis	This property defines whether to use the results of the current analysis as loading or as an initial condition in a subsequent downstream analysis. Supported analysis types and the supported downstream systems are described below. Coupled Field Static Options include None (default) and Prestressed Analysis. If a Coupled Field Static analysis is used to provide Pre-Stress effects, this property automatically defaults to the Prestressed Analysis setting. It can provide Pre-Stress effects for the following analysis types: Pre-Stressed (Full) Coupled Field Harmonic Pre-Stressed Coupled Field Modal Harmonic Response Options include None (default) and Structural Optimization. If you select Structural Optimization, the application automatically sets other Analysis Settings properties to specific read-only settings. Such as the Multiple Steps property, the Solution Method property (Mode Superposition), Output Controls properties, and On Demand Expansion property. If you link a Harmonic Response analysis to a downstream Structural Optimization analysis, this property automatically defaults to the Structural Optimization setting, becomes read-only, and the same automatic actions as stated above apply. Unlinking these analyses reverts all automatic read-only settings. Modal Options include None (default), MSUP Analyses, Structural Optimization, or MSUP & Structural Optimization. When linked to a supported analysis type (Harmonic Response or Random Vibration (PSD) or Response Spectrum), this property automatically defaults to the MSUP Analyses setting. Note: A Modal analysis is a prerequisite for the following analysis types: Random Vibration (PSD) Response Spectrum If a Modal analysis is linked with a Structural Optimization analysis, this property automatically defaults to the Structural Optimization setting. If a Modal analysis is linked with a Harmonic Response, or a Random Vibration (PSD), or a Response Spectrum analysis and a Structural Optimization analysis, this property automatically defaults to the MSUP & Structural Optimization setting. Static Structural Options include None (default), Prestressed Analysis, Structural Optimization, and PreStressed & Structural Optimization. If a Static Structural analysis is used to provide Pre-Stress effects, this property automatically defaults to the Prestressed Analysis setting. It can provide Pre-Stress effects for the following analysis types: Pre-Stressed (Full) Harmonic Response Pre-Stressed Modal Pre-Stressed Eigen Value Buckling Note: A Static Structural analysis is a prerequisite for Eigenvalue Buckling analysis. If a Static Structural analysis is linked with a Structural Optimization analysis, this property automatically defaults to the Structural Optimization setting. If a Static Structural analysis is linked with a Modal analysis or a Harmonic Response analysis and a Structural Optimization analysis, this property automatically defaults to the PreStressed & Structural Optimization setting. Substructure Generation Options include None (default) and Ansys Rigid Dynamics (Beta) (visible when you activate Beta Options). When you select the Ansys Rigid Dynamics (Beta) option, the application automatically includes the additional files necessary to perform a downstream Rigid Dynamics analysis in the exported file.
Scratch Solver Files Directory	This is a read-only indication of the directory where a solve "in progress" occurs. All files generated after the solution is done (including but not limited to result files) are then moved to the Solver Files Directory. The files generated during solves on My Computer or files requested from RSM for postprocessing during a solve remain in the scratch directory. For example, an early result file could be brought to the scratch folder from a remote machine through RSM during postprocessing while solving. With the RSM method, the solve may even be computed in this folder (for example, using the My Computer, Background Solve Process Settings). The scratch directory is only set for the duration of the solve (with either My Computer or My Computer, Background). After the solve is complete, this directory is set to blank. As desired, you can specify a unique disk location for this directory using the Scratch Solver Files Directory option in the Analysis Settings and Solution category of the Options preference settings. Specifying a different disk location for the scratch files enables you take advantage of a faster disk drive. The use of the Scratch Solver Files Directory prevents the Solver Files Directory from ever getting an early result file.
Save MAPDL db	Options include No (default) and Yes. Some Future Analysis settings will require the database file to be written. In these cases this field will be set to Yes automatically.
Contact Summary	This property enables you to control where contact pair data is written during the solution process, either to the solver output file or to a contact output file. This ability enables you to limit the contact data written to the solver output file. Property options include Program Controlled (default), Solver Output, and CNM File. If your model includes more than 100 contact pairs, the Program Controlled option automatically writes contact pair data to a contact output text file named file.cnm (refer to the CNTR,OUT,YES command), otherwise the data is written to the solver output file. The Solver Output option writes the data as normal to the solver output file. The CNM File option writes contact pair data to file.cnm regardless of the number of contact pairs in your model.
Delete Unneeded Files	Options include Yes (default) and No. If you prefer to save all the solution files for some other use you may do so by setting this field to No. Important: When you are 1) using the Mechanical APDL solver, 2) have the Distributed solve option selected (default), and 3) this property is set to Yes (required), the application automatically executes the Mechanical APDL command /FCLEAN. This command deletes all unnecessary distributed files from the scratch directory. In addition to this property needing to be set to Yes, the Future Analysis property (described above) must be set to None for the command to execute properly. These requirements apply to each analysis system included in your project. The action of deleting unnecessary distributed files is especially useful for solutions being performed on a remote machine because it eliminates the need to download potentially large files that serve no specific purpose for the postprocessing of your analysis. Limitation: For Static Structural and Transient Structural analyses, setting this property to Yes automatically sets the Restart Controls property Retain Files After Full Solve property to Yes (the default is No) and the application does not execute the /FCLEAN command. However, changing the Delete Unneeded Files property from Yes to No DOES NOT automatically reset the Retain Files After Full Solve property (to No). If you are using a Samcef or ABAQUS solver interface for your analysis, the Solver Files Name setting controls the name of the files generated in the analysis directory. By default, this setting is the name of the solver being used ("samcef" or "abaqus").
Nonlinear Solutions	Read only indication of Yes or No depending on presence of nonlinearities in the analysis.
Solver Units	You can select one of two options for this property: Active System: This options instructs the solver to use the currently active unit system (determined via the Units option in the Tools group of the Home tab.) for the very next solve. Manual: This option enables you to select the unit system for the solver to use by allowing them access to the second field, "Solver Unit System".
Solver Units System	If Active System is chosen for the Solver Units field, then this field is read-only and displays the active system. If Manual is chosen for the Solver Units field, this field is a selectable drop-down menu. If a Magnetostatic analysis is being performed, the field is read only because the only system available to solve the analysis is the mks system. For the following analyses, only the mks and umks solver unit systems are supported and can be selected: Electric Thermal Electric Coupled Field (only when the Electric physics property is set to Yes on the Environment)
Max Num of Intermediate Files	This property is for Structural Optimization analyses only. It specifies the number of files you wish to retain. A value of `1` indicates that the generated file is overwritten each iteration. The default value for the property is set to the text string "All Iterations" that equals a setting of zero (`0`). This setting saves the intermediate topology files for all iterations solved. Note: The animation of the Topology Density results and Topology Elemental Density results is based on the number of intermediate results computed and saved during solution. The computation of results is driven by Store Results At property of the Output Controls and the intermediate results saved is driven by this property. You can change the default setting for this property using the Max Num Of Intermediate Files property under the Analysis Data Management (Structural Optimization) category of the Options > Analysis Settings and Solution preference.