Solver Settings in Creo Ansys Simulation
Default solver settings are available when you open the application. Most of the time you can use the default settings but for some advanced simulations you might need to adjust the default solver setting to improve performance and improve the chances of convergence. You can change settings for a particular simulation study. Click > 
Simulation Setup to open the Solver Settings dialog box. The following settings are available:
Simulation Setup to open the Solver Settings dialog box. The following settings are available:General Solver Settings
The default values of these settings are defined on the Simulation page of the Creo Parametric 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. |
For more details refer to this topic.
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. Warn—This is the default value. The solver warns about gaps or overlaps at contact interfaces before solving.
For more details refer to this topic.
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.
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. |
For more details refer to this topic.
The configuration option creo_ansys_n-r_method controls the default value of this option.
• Large Deflection—Specifies whether solver calculations must consider large deflections and rotations, or assume there are only small deflections in the model. This option is only available for structural simulation studies. It has the following options:
◦ Off—By default this is the selected option. The solver calculations assume there are no large deflections in the model.
◦ On—Select this option so that solver calculations always assume that there are large deflections and rotations in the model.
• Damping—Specify settings related to damping in the structure.
◦ Direct Input—Specify the stiffness coefficient, mass coefficient and numerical damping for the model. Specify a value of 0 for all options to simulate an undamped analysis. For a damped system specify a non-negative number.
◦ Damping Vs Frequency—Specify damping at a certain dominant frequency for the model. In this case specify damping ratio, stiffness coefficient, and numerical damping.
Stiffness coefficient = 2 * damping ratio / ( 2 * pi * frequency in Hertz)
◦ Stiffness Coefficient(Beta Damping)—A coefficient value that is a multiplier for the stiffness matrix.
◦ Mass Coefficient(Alpha Damping)—A coefficient value that is a multiplier for the mass matrix.
Frequency—Specify the dominant frequency at which damping is considered. The value must be positive.
◦ Damping Ratio—The ratio of actual damping to the critical damping for the frequency specified as the dominant frequency. This is required when you select Damping Vs Frequency as the type of damping.
◦ Numerical Damping—Numerical Damping is also referred to as amplitude decay factor (γ). Numerical damping controls the numerical noise produced by the higher frequencies of a structure. Specify a non-negative number.
• Inertia Relief—Specifies whether to use inertia relief or the constraints defined for the study. This option is only available for structural simulation studies. It has the following options:
◦ Off—By default this is the selected option. The solver uses the constraints defined in the model.
◦ On—Select this option for the solver to use inertia relief and ignore the constraints defined in the model.
The configuration option creo_ansys_use_inertia_relief 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.
This option is only available for modal studies.
• Simulation Steps—Specifies the number of simulation steps for a solution. These settings are optional and are applicable to structural simulation studies only.
Step Options
Step Options—Defines the solution options for each step.
• Simulation Step—Selects Step number as Step 1, Step 2 etc. It depends on the number of steps defined in Simulation Steps.
• Step Duration—Sets the time duration of each step. The total analysis time is the sum of all the step duration of all the simulation steps.
• Substepping—Controls substep settings.
• Method—Select one of the following methods:
◦ Automatic—Allows the solver to control the selection of substeps.
◦ Manual—Specifies the number of substeps manually.
◦ Adaptive—Specifies initial, minimum, and maximum substeps, and varies the solution stepping within this range.
For the manual or adaptive methods you can also specify whether the load increments between substeps is based on one of the following options:
▪ No. of substeps—Load increments for a substep are based on the number of substeps. This is the default value.
▪ Time—Load increments for a substep are based on time.
◦ Initial Substeps—Defines the initial number of substeps. Specify a positive integer as the value. The default value is 1. Available for Manual and Adaptive methods of substepping.
◦ Minimum Substeps—Defines the minimum number of substeps. Specify a positive integer as the value. The default value is 1. Available only for Adaptive method of substepping.
◦ Maximum Substeps—Defines the maximum number of substeps. Specify a positive integer as the value. The default value is 10. Available only for Adaptive method of substepping.
Force Convergence Tab
Force Convergence—This option is for structural simulations only. For thermal studies the tab is named Heat Convergence.
• Method—Select one of the methods for force convergence in your solution:
◦ Automatic—Allows convergence values to be calculated automatically.
◦ Manual—Enables you to specify convergence values manually.
◦ Off—Doesn’t check for convergence of the solution.
• Tolerance—Specify tolerance as a percentage value.
• Ref Value—Specify real numbers with a default value of 1.
• Tolerance times Ref Value determines the convergence criterion.
Reset—Click the Reset button to restore the default settings for all the options in the Solver Settings dialog box.