Thermal-Fluid-Structural Analyses using System Coupling

Thermal-fluid-structural coupling between Mechanical and another participant system (such as Fluent) are supported, with an expert option used in Mechanical to enable the data transfers. For this analysis, the Mechanical model needs to be created using the Static Structural or Transient Structural system, and you also need to use the appropriate Coupled Field Elements (SOLID226 and SOLID227).

To do a thermal-fluid-structural analysis, in Mechanical’s Details of “Fluid Solid Interface”, you have to set Definition>Data to Transfer [Expert]>System Coupling Data Transfers. This expert setting allows the fluid solid interface regions to participate in force, displacement, and thermal couplings through the System Coupling service.

For a thermal-fluid-structural analysis, the coupled field elements SOLID226 and SOLID227 (KEYOPT(1)=11) need to be used in Mechanical because they have the appropriate degrees of freedom. The element SOLID226 replaces any SOLID186, and the element SOLID227 replaces any SOLID187. To select the proper coupled field elements into your structural analysis, follow these steps to insert the correct Commands objects:

  1. In your Workbench Project Schematic, update your structural system’s Setup cell and locate the ds.dat file. Or, you can use Tools>Write Input File to write out this file.

  2. Open the ds.dat file in a text editor and search for “et,” to locate the element types for each body. In the example below, the body named "fea" has SOLID186 elements. Bodies may have more than one element type ("fea" may also contain SOLID187). Make sure to keep searching until you have identified all of the element types associated with each solid body.

    Figure 16:  Example of a search for element types in a ds.dat file

    Example of a search for element types in a ds.dat file

  3. In Mechanical’s Outline tree, below Geometry, right-click the solid body and insert a Command. Add the appropriate ET commands under each solid body, replacing SOLID186 with SOLID226, and SOLID187 with SOLID227.

    For the case shown in Figure 17: Example of element types in multiple solid bodies, the commands that you would use for each body are:

    • For Body 1 “Pipe”, the command is: et,matid,226,11

    • For Body 2 “Clamp”, the command is: et,matid,227,11 and et,matid+1,226,11

    • For Body 4 “Support”, the command is: et,matid,226,11

    Note that matid and matid+1 are used to refer to the element type number.

    Figure 17:  Example of element types in multiple solid bodies

    Example of element types in multiple solid bodies

  4. In the Outline tree, below Static or Transient analysis, insert a Commands object to define the thermal boundary conditions.

  5. Create Named Selections for regions that require thermal boundary conditions, then refer to these named selections in the Commands object that you created in step 4. Within your Commands, the IC command sets the initial temperature. The SF command is used to define convection, heat flux, and radiation loads. The D command is used to set a temperature constraint on the named selection.

In your thermal-fluid-structural analysis using coupled field elements:


Release 18.2 - © ANSYS, Inc. All rights reserved.