Settings for Creo Ansys Simulation
Before you begin running simulation studies you can configure Creo Ansys Simulation to use some default global settings. Perform the following steps from Creo Ansys Simulation or from Creo Parametric.
1. Click > to open the Creo Parametric Options dialog box.
2. Click Simulation from the left pane to display the Set Simulation Options page.
3. You can change any of the following settings or view and retain the default values. Each of these settings also has a corresponding configuration option that you can modify to change the default setting:
a. Click Solver Settings to open the Solver Settings options dialog box.
▪ Solver Type—Select the default type of Ansys solver to be used:
▪ Automatic—This is the default value. Selects the most appropriate solver for the model.
 |
This option is recommended, unless directed to change to address specific convergence or performance issues.
|
▪ Direct—Obtains the solution by direct stiffness matrix inversion.
▪ Iterative—Obtains the solution by approximating and iterating.
▪ Supernode—This option is only used for modal analyses. It uses a mathematical subtraction algorithm to obtain all the modes at the same time. It is useful for calculation on nodes in the known frequency range.
▪ Subspace—This option is only used for modal analyses. It uses the subspace Eigensolver method that utilizes symmetric matrices for obtaining a solution.
The configuration option creo_ansys_solver_type controls the default value of this option.
▪ Contact Gap/Overlap—Selects the default behavior of the solver when it detects gaps or overlaps at contact interfaces. Choose one of the following options:
▪ Warn—This is the default value. The solver warns about gaps or overlaps at contact interfaces before solving.
▪ Fix—The solver attempts to fix gaps and overlaps at contact interfaces before solving the study.
▪ Allow—The solver considers gaps or overlaps as intended design and allows them in the model when solving.
The configuration option creo_ansys_contact_gap_behavior controls the default value of this option.
▪ Newton Raphson method—Specifies options for the Newton-Raphson method of convergence. Select one of the following options:
▪ Automatic—Default Value. Allows the solver to select the best solution.
|
|
This option is recommended, unless directed to change to address specific convergence or performance issues.
|
▪ Full—The solver uses the full Newton-Raphson procedure, in which the stiffness matrix is updated at every equilibrium iteration.
▪ Modified—The solver uses the modified Newton-Raphson technique, in which the tangent stiffness matrix is updated at each substep. The matrix is not changed during equilibrium iterations at a substep. This option is not applicable to large-deformation analyses. Adaptive descent is not available.
▪ Initial stiffness—The solver uses the initial stiffness matrix in every equilibrium iteration. This option can be less likely to diverge than the full option, but it often requires more iterations to achieve convergence. It is not applicable to large-deformation analyses. Adaptive descent is not available.
▪ Unsymmetrical—The solver uses the full Newton-Raphson procedure, in which the stiffness matrix is updated at every equilibrium iteration. In addition, it generates and uses unsymmetrical matrices that you can use for any of the following:
▪ When you define an unsymmetrical material model, you need this method to fully use the property that you defined.
▪ If you run a contact study, an unsymmetrical contact stiffness matrix fully couples the sliding and the normal stiffnesses. You should first try the Full method, then try this method only if you experience convergence difficulties. (Using an unsymmetrical solver requires more computational time to obtain a solution than a symmetric solver.)
The configuration option creo_ansys_n-r_method controls the default value of this option.
▪ Normal Modes—Specifies the number of natural frequencies to solve for in a modal simulation study. The default is to extract the first six natural frequencies.
The configuration option creo_ansys_normal_modes controls the default value of this option.
b. Solve for all result types—To make all the advanced result types available by default select this check box for all advanced result types to be available. By default, this check box is not selected and strain and nodal load results are not available.
The configuration option creo_ansys_all_results_visible controls the default value of this option.
c. Creo Ansys simulation run folder—Specifies the location to store the temporary solver data. The default run folder is $TMP\ where $TMP is the environment variable TMP for a user.
You can also specify the default location in the config.pro file using the configuration option creo_ansys_run_folder.
|
|
The full path to this location must not include Unicode characters and can have a maximum length of 248 characters only.
|
d. Creo Ansys simulation cache folder—Specifies the location to store solver data when you save the model. The default location is $APPDATA\Creo\CreoAnsys where $APPDATA is the environment variable $APPDATA for a user.
You can also specify the default location in the config.pro file using the configuration option creo_ansys_cache_folder.
|
|
Solver and simulation data that is saved to the cache folder can grow to a very large size over a period of time. The $APPDATA location is not cleared automatically either by the operating system or the software so it is a good practice to specify a location other than $APPDATA\Creo\CreoAnsys as the default location to store saved solver and model data and to clear it periodically.
|
4. Click OK. You are prompted to save the changes to the config.pro file. If you do not save the changes to the config.pro file then they are only valid for the session, and revert to the previous or default values when you close the session.