Use the workflow below to perform a submodeling analysis using linked thermal systems. You should review the Data Transfer Mesh Mapping content in Appendix C of the Help. This section describes the various Details view properties associated with the loading types for the submodeling feature. Refer to this section as needed during your analysis.
Supported Boundary Conditions
Thermal submodeling analyses support the Imported Temperature only.
Thermal Analysis Submodeling Workflow
On the Workbench Project page, create and complete (solve) a steady-state thermal or transient thermal analysis. Perform all of the steps to set up and analyze the model. Specify mesh controls, boundary conditions, and solution settings as you normally would and solve the analysis.
To easily identify this initial model, this example uses the name "Coarse" to identity the upstream system. This does not mean that the mesh refinement is coarse, only that it is relatively coarse compared to the "Submodel."
Create a new Steady-State Thermal or Transient Thermal analysis on the Project page. Link the Solution cell of the upstream onto the Setup cell of the downstream system. As required, you can also link the Engineering Data and Geometry cells.
Note:You can add a template for the linked thermal systems by creating your own template.
Data can be transferred from a 2D coarse model to a 3D submodel. The settings for 2D projection of target mesh nodes can be specified in Appendix B: Data Transfer Mapping and Validation.
Double-click the downstream system's Setup cell to open Mechanical. The application automatically adds a Submodeling object to the system's tree. This object references the upstream analysis' Solution object in parenthesis, for example, Submodeling "(A6)".
An imported temperature object is automatically inserted under the Submodeling folder to represent the transfer. To add additional Imported Temperature objects, right-click the Submodeling folder and select the appropriate load from the context menu.
Now, you need to select the appropriate cut-boundaries from the geometry using either the Geometry or the Named Selection scoping option.
The Imported Temperature boundary condition supports Face, Edge, and Node selections for 3D solids and Edge and Node selections for 2D shells.
Note: You cannot mix the scoping of surface bodies with other geometry types.
The application automatically populates the Transfer Key property. Options include:
- Shell-Shell
The application selects this option for a shell-based geometry in the upstream system.
- Solid-Solid
The application selects this option for a solid body geometry in the upstream system.
- Shell-Solid
You may select this Transfer Key option for Shell-to-Solid submodels.
- Beam-Shell/Solid
The application selects this option for a beam-based geometry in the upstream system.
Note:When you set the Transfer Key property to or , only shell bodies are selected from the upstream analysis.
When the Transfer Key is set to , only beam bodies are selected from the upstream analysis.
Mapping Validation is not supported when the Transfer Key property is set to or .
If you are using the Material Assignment feature on source bodies that are different (shell and beam), you could experience mapping errors. The application may skip a source body during the mapping process. To address this issue, use the feature on the bodies individually – do not mix body types.
The application only considers beam and shell section type elements from the source data. It ignores all other section types.
The range of data displayed in the graphics window can be controlled using the Legend controls options. See Imported Boundary Conditions for additional information.
As needed, modify Details view properties. See Appendix C for additional information.
Right-click the Imported Load object and click Import Load to import the load. When the load has been imported successfully, a plot of the mapped values will be displayed in the Geometry window.
To activate or deactivate the load at a step, highlight the specific step in the Graph or Tabular Data window, and choose Activate/Deactivateat this step!
See Activating and Deactivating Loads for additional rules when multiple load objects of the same type exist on common geometry selections.
Define any other loads and boundary conditions, specify load step options, and obtain the submodel solution.
The final step is to verify that the cut boundaries of the submodel are far enough away from the concentration. You can do this by comparing results (stresses and so on) along the cut boundaries with those along the corresponding locations of the coarse model. If the results are in good agreement, it indicates that proper cut boundaries have been chosen; otherwise, you will need to recreate and reanalyze the submodel with different cut boundaries further away from the region of interest.
Note: If the upstream (Coarse) system is modified and re-solved after importing the load, a refresh operation on the Submodel system’s Setup cell is required to notify Mechanical that source data has changed and re-import is required. Alternatively, the source data can be refreshed using the right-click operation on the Submodeling folder and choosing the Refresh Imported Load option.