This is the workflow for performing a submodeling analysis with linked thermal systems:
From the toolbox, drag and drop a transient or steady-state thermal template onto the project schematic. Perform all of the steps to set up and analyze the initial model. Specify mesh controls, boundary conditions, and solution settings as you normally would and solve the analysis. To easily identify this initial model, it is referred to as the coarse model. This does not mean that the mesh refinement is coarse, only that it is relatively coarse compared to the submodel.
Drag-and-drop a Steady-State Thermal or Transient Thermal template onto the project schematic. Share the Engineering Data and Geometry cells if required and then drag the Solution cell of the upstream onto the Setup cell of the downstream system.
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.
Double-click the downstream systems Setup cell. In the Mechanical application, a Submodeling folder is automatically added into the system's tree.
An imported temperature object is automatically inserted under the Submodeling folder to represent the transfer. To add additional Imported Temperature objects, click the Submodeling folder to make the Environment toolbar available, or right-click the Submodeling folder and select the appropriate load from the context menu.
Select appropriate cut-boundaries for transferring temperatures or body selections for transferring temperatures in the Details view of the Imported Load object using the Geometry or Named Selection scoping option.
Note: Mixing of scoping on surface bodies with other geometry types is not allowed.
The Transfer Key is automatically selected in the details view based on scoping. For scoping on surface bodies, Shell-Shell Transfer Key is selected. For scoping on solids, Solid-Solid Transfer Key is selected by default. Change it to Shell-Solid for shell to solid submodeling.
The Source Bodies option in the Details view enables you to select the bodies, from the upstream analysis, that make up the source mesh when mapping the data. You can choose one of the following options:
All: The source mesh in this case will comprise of all the bodies that were used in upstream analysis. For cases where the source values are significantly different at the boundaries across two or more bodies, the interpolation may need to be performed separately on each geometry to ensure that the mapped values match the source.
Manual: This option enables you to select one or more source bodies to make up the source mesh. The source body selections are made in the Material IDs field by entering the material IDs that correspond to the source bodies that you would like to use. Type material IDs and/or material ID ranges separated by commas to specify your selection. For example, type 1, 2, 5-10. The material IDs for the source bodies can be seen in the Solution Information Object of the source analysis. In the example below, text is taken from a solver output:
***********Elements for Body 1 "coil" *********** ***********Elements for Body 2 "core" *********** ***********Elements for Body 3 "bar" ************
The body 'coil' has material ID 1, body 'core' has material ID 2, and body 'bar' has material ID 3.
Note: For Shell-Shell and Shell-Solid Transfer Key, only shell bodies are selected from the upstream analysis.
For Solid-Solid Transfer Key, the values on the middle shell plane of shell bodies are used for mapping.
You can transform the source mesh used in the mapping process by using the Rigid Transformation properties. This option is useful if the source geometry was defined with respect to a coordinate system that is not aligned with the target geometry system.
When scoped on surface bodies, you can control the effective offset and thickness value at each target node of the surface bodies, and consequently the location used during mapping, by using the Shell Thickness Factor property. See Structural Submodeling Workflow for more details.
Change any of the columns in the Data View tab as needed:
Source Time: The time at which the data will be imported from the coarse analysis.
Analysis Time: Choose the analysis time at which the load will be applied.
Note: The Data View can automatically be populated with the source and analysis times using Source Time property in the Details View. Use All to import data at all times in the source analysis, or Range to import data for a range specified by a Minimum and a Maximum.
You can define multiple rows in the Data View tab to import source data at multiple times and apply them at different analysis times. If multiple rows are defined in the Data View, it is possible to preview imported load vectors/contour applied to a given row or analysis time in the Data View. Choose Active Row or Analysis Time using the By property under Graphics Controls in the details of the imported load and then specify the Active Row/Analysis Time to preview the data.
Note: If the Analysis Time specified by the user does not match the list of analysis times in the Data View, the data is displayed at the analysis time closest to the specified time.
You can modify the Mapper Settings to achieve the desired mapping accuracy. Mapping can be validated by using Mapping Validation objects.
Note: Mapping Validation is not supported for Shell-Solid Transfer Key.
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.
Note: The range of data displayed in the graphics window can be controlled using the Legend controls options. See Imported Boundary Conditions for additional information.
To activate or deactivate the load at a step, highlight the specific step in the Graph or Tabular Data window, and choose Activate/Deactivate at this step!
See Activation/Deactivation of 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.
For more information, see Imported Temperature.