Solution Setup (Thermal)

You must add at least one solution setup to each Mechanical design. The solution setup for a Thermal analysis includes the following settings:

[General Tab]

• Name: The default name is Setupx, where x is a numeric value incremented for each solution setup that you add to the design. You can customize the name of each setup as desired.
• Enabled: This option is selected by default. Deselect the option to prevent the setup from being solved when you click the Analyze All command.
• Solver Type: Specify the solver to use, or let the program choose the solver. The choices are:
• Program Controlled: This is the default setting, which is recommended for most cases. The application selects the optimal solver.
• Direct
• Iterative
Note:

Consult the Ansys Mechanical User's Guide (specifically, Configuring Analysis Settings > Analysis Settings for Most Analysis Types > Solver Controls) for more information about the available solver choices.

• Transient Setup: For Transient Thermal solutions, you must specify the Start time, Stop time, and Time Step of the simulation in the Transient Setup section:



Optionally, click Time variation preview to see a plot of time-varying boundaries or constraints:



• Stepping: Specify whether stepping is enabled, or let the program choose. Stepping is the process of dividing the applied loads (excitations and boundaries) into smaller increments to make solution convergence easier. In the context of steady-state thermal analyses, only the loads are divided, not time increments, since the time to achieve steady-state conditions (that is, thermal equilibrium) is unknown.

The Stepping options are:

• Program Controlled: This is the default setting, which is recommended for most cases. The application determines the stepping settings.

There are no additional settings to specify in the General tab for Steady-State Thermal solutions when this Stepping option is selected:



• Off: Program controlled or user-defined automatic stepping is disabled. However, you can still specify a fixed number of calculation Substeps (steady-state or transient solutions) or Time Substeps (transient solutions only). When this option is selected, the following additional setting appears in the dialog box:

   

• # Substeps: The number of substeps to solve for a steady-state solution or the number to solve per requested time step in a transient solution. In a steady-state solution, you can think of a substep as a load division for all assigned boundaries and excitations. For example, if you apply a 6 watt heat generation excitation, and you specify two substeps, the solver increments the generated heat by 3 watts for each calculation substep. That is, the solution is calculated at 3 W and 6 W of heat input. The applied thermal loads (boundaries and excitations) are divided according to the number you specify and solved as intermediate steps and a final step.

Substeps can have a similar effect for transient solutions if a thermal source or load is in transition at the time step being divided into smaller pieces. This effect combined with the shorter calculation time increment can improve the ease of solution convergence. (See Note below.)

• Time Substeps: In a transient solution, time substeps reduce the duration of the default solution Time Step specified in the Transient Setup section. The effect is similar to that of specifying substeps except that you are directly defining the calculation time increment rather than the number of substeps. Any thermal sources or loads that are in transition at the time of a given solution step are analyzed in smaller, partial changes in magnitude. This load change reduction, and the shorter calculation time increment can lead to easier convergence of the solution. (See Note below.)
• On: User-defined stepping is enabled. When this option is selected, the following additional settings appear in the dialog box:

   

• Initial: The initial number of substeps to run, or initial substep time increment (for transient solutions only).

For steady-state solutions: The applied thermal loads (boundaries and excitations) are divided according to the initial number of substeps to represent a "bite-sized" portion of the full thermal load. The default Initial substeps value is 1, in which case the full thermal load is applied initially. This number should be greater than or equal to the Min number of substeps (next bullet).

For transient solutions: The default Initial time substep is 0.01s. Alternatively, you can choose to specify the initial number of substeps. in which case the default is 100.

• Min: The minimum number of substeps to be solved or the shortest substep duration (for transient solutions only). The default is 1 for steady-state solutions and either 0.003s or, alternatively, 10 substeps for transient solutions.

If no convergence problems are encountered, the solver can reduce the number of substeps to something between the Initial and Minimum values, essentially increasing the size of the load step. For transient solutions using the Time option, the duration of the substep is increased to something between the Initial and Maximum values to achieve the same effect.

If you specify Min greater than Initial, the solver will reset Min to be equal to Initial. Therefore, the value you enter for Min should be less than or equal to the Initial number, or duration, of substeps you define.

• Max: The maximum number of substeps to solve or the maximum substep duration (for transient solutions only). The default is 10 for steady-state solutions and either 0.1s or, alternatively, 100 substeps for transient solutions.

More substeps than specified by the Initial setting (or substeps with a greater duration) are solved only if convergence problems are encountered. A greater number of calculation substeps (or a shorter substep duration) corresponds to smaller load steps, making convergence easier.

Note:
• While results are produced by the solver for each calculation substep, these intermediate results are not available for reporting in the Ansys Electronics Desktop application. Only the final solution results (for a steady-state solution) or results at the requested Time Step interval (for transient solutions) are available for post processing (see Save Fields Tab below).
• In the context of a steady-state thermal analysis, you are not dividing the analysis into periods of time. You are only specifying load substeps, each of which has a steady-state solution of unknown time.
• In the absence of nonlinear materials, radiation (which is highly nonlinear), and time-dependent or temperature-dependent excitations or boundaries, thermal analyses is likely to converge in a small number of steps without difficulty. Therefore, we recommend that you use the Program Controlled option, which allows up to ten substeps and as few as one.

[Advanced Tab]

Use this tab to set up Mesh Linking when desired. Additionally, for transient thermal analyses, use this tab to set options for transient restart analyses.

[Convergence Tab]

This tab contains optional solver controls and tolerance values for temperature and heat convergence.

[Initial Conditions Tab]

Use this tab to define the initial object temperature the solver is to use for the analysis. An appropriate initial temperature can shorten the solution time.

[Save Fields Tab] (Transient Thermal Solutions only)

Use this tab to choose whether to save fields data and at what frequency to save the data when wanted.

How to Set Up a Thermal Solution:

1. Use one of the following three methods of accessing the thermal solution settings:
• On the Simulation ribbon tab, click Setup.
• Right-click Analysis in the Project Manager and choose Add Solution Setup.
• Using the menu bar, click Mechanical > Analysis > Add Solution Setup.
2. Optionally, change the Name and any of the other default general settings (Solver Type, Stepping or Transient Setup options) that have been previously described in this topic.
3. Optionally, click HPC and Analysis Options to change any of your high performance computing configurations or options.
4. Optionally, specify settings for importing a mesh from another design or project. (See Mesh Linking.)
5. Optionally, specify user-defined options for temperature and heat convergence.
6. Optionally, specify an initial condition (starting temperature) for the solution.
7. Optionally, for transient thermal solutions, specify whether to save fields and how frequently to save them.
8. Click OK.

The setup appears under Analysis in the Project Manager: