The coupling involves solving an electromagnetic problem in Maxwell, and mapping the resulting volumetric and/or surface loss information into Fluent. Volumetric loss is mapped onto the cell zones as a heat source (load) at the cell centroids that is then added to the energy equation. Surface loss is applied to the adjacent cells of the solid zones that contribute to the source terms of these cells.
Note: Surface loss is highly concentrated near the surface of the solid zone, so it is recommended that you have a layer of good quality hexahedral or prism mesh elements located where surface loss occurs.
Note: You can analyze the results of volumetric/surface losses using the following postprocessing variables:
Volumetric loss: Temperature EM Source ()
Surface loss: Temperature EM Surface Source
()
The overall workflow for an Maxwell-Fluent analysis is as follows:
Create and solve the electromagnetic application using Maxwell.
Drag and drop a Fluent–based system and import a case or mesh file into Fluent, and then double-click the Setup cell to start Fluent.
Note: If you import a mesh into Fluent that was generated using non-SI units, then you should scale and/or translate the mesh before you perform any coupling with Maxwell.
Drag and drop the cell of the Maxwell system onto the Setup cell of Fluent system to enable the data transfer.
Update the Solution cell of the Maxwell system.
Refresh the Setup of Fluent system.
Specify the EM settings in Fluent (File/EM Mapping).
Set up the Fluent analysis as you normally would (for example, specify boundary conditions, solution settings, and so on).
Solve the Fluent analysis.
During EM mapping, Fluent automatically turns on the energy model, if you have not already done so.
Note: In 2D axisymmetrical cases only, Maxwell uses the RZ (or XZ) plane while Fluent uses the XY plane by default. Therefore, when you export a geometry from Maxwell, you need to rotate the geometry in order for Fluent to mesh the geometry before EM mapping can take place properly. This is not a concern for regular 2D or 3D cases. If you use ANSYS DesignModeler, rotate the geometry exported from Maxwell by performing the following steps:
Define a new plane based on the XY plane, applying a 90 degree rotation along the X axis, and a 90 degree rotation along the Y axis.
Move the geometry from the XY plane to the new plane.
If you use SpaceClaim (Windows only), follow the steps below:
Make sure that the world origin is displayed ( > > > ).
In the Design ribbon tab, select the Orient tool (Assembly group).
Select an edge of the geometry you want to rotate and then select a global axis.
The geometry will be rotated so that the selected edge is aligned along the selected global axis.