When you export a mesh file to Ansys Fluent mesh format ( from the Meshing application main menu, then Fluent Input Files), a mesh file with the extension .msh is created. The exported mesh file is suitable for import into another product such as Ansys Fluent, or into Ansys Fluent Meshing outside of Ansys Workbench. For more control over the input file, refer to Meshing Options on the Options Dialog Box.
If the mesh file you export contains quadratic elements, all midside nodes will be dropped during export. That is, all element types will be exported as linear element types for Ansys Fluent.
An orientation check/correction will be performed for 3D geometry models exported as 2D mesh such that all 2D cells will have the same orientation. You do not need to manually correct the orientation of the geometry face(s).
When the mesh file is exported to Ansys Fluent mesh format, the material properties of the bodies/parts in the model must be translated to proper continuum zone types for use in Ansys Fluent. To provide this information to Ansys Fluent, the following logic is used:
If Physics Preference is set to and you do not use either of the methods described in steps 2 or 3 below to explicitly assign a body/part to be either solid or fluid, all zones are exported to Ansys Fluent mesh format as FLUID zones by default.
Note: An exception to the above involves models that include an enclosure. If you used the Enclosure feature in the Ansys DesignModeler application, the enclosure body will be assigned a continuum zone type of FLUID by default.
For models created/edited in the DesignModeler application, a Fluid/Solid material property can be assigned to a solid body or a multibody part (if the multibody part contains at least one solid body). This material assignment appears under Details of Body in the Details View of the DesignModeler application.
For multibody parts, you can change the material property for all bodies in one operation in the DesignModeler application by modifying the Fluid/Solid property for the multibody part and the modification will propagate to any solid bodies in the part. Similarly, you can use the DesignModeler application to modify the Fluid/Solid property for a solid body that belongs to a multibody part, and the Fluid/Solid property for the multibody part will be modified accordingly.
When exported to Fluent Meshing format, a body/part with a material property of will be assigned a continuum zone type of SOLID and a body/part with a material property of will be assigned a continuum zone type of FLUID. This setting in the DesignModeler application overrides the default behavior described in step 1.
Note: Refer to Figure 5: Multibody Part Containing All Fluid Bodies in the DesignModeler Application for an example that illustrates where to set the Fluid/Solid material property in the DesignModeler application.
Finally, the Fluid/Solid material property setting in the Meshing application is considered. This material assignment appears in the Details View of the Meshing application when a prototype (Body object) is selected in the Tree Outline. Similar to the DesignModeler application feature described in step 2, the Meshing application lets you change the Fluid/Solid material property for a body.
When exported to Ansys Fluent mesh format, a body with a material property of will be assigned a continuum zone type of SOLID and a body with a material property of will be assigned a continuum zone type of FLUID. This setting in the Meshing application overrides any assignments that were made based on the default behavior described in step 1 or the Fluid/Solid setting described in step 2.
Note: If there are multiple continuum zones or boundary zones of the same type in the DesignModeler application or the Meshing application, each zone name in the exported Ansys Fluent mesh file will contain the necessary prefix and an arbitrary number will be appended to the name to make it unique. Refer to Examples of Fluent Mesh Export: An Alternative to Using a Fluid Flow (Fluent) Analysis System for an example that illustrates multiple zones of the same type.
For related information, refer to:
Note:
Contact regions are said to be “overlapping” when the same entity (face or edge) is a member of more than one contact region or when multiple contact regions share the same geometry. Ansys Fluent does not support overlapping contact regions. For part-based meshing only, if you are exporting a mesh into the Ansys Fluent format and overlapping contact regions are detected, the software will attempt to combine the regions. If it is unable to combine them, the export will fail and you must resolve the overlapping contact regions manually before proceeding. You can use the Check Overlapping Contact Regions option to identify the problematic contact regions. For details, see Resolving Overlapping Contact Regions.
If you are performing a 2D analysis and intend to export to Ansys Fluent, you should disable the Auto Detect Contact On Attach option to avoid problems that may otherwise occur upon export. You can access this option by selecting from the Ansys Workbench main menu, and then selecting either the Mechanical or Meshing category as appropriate. The option is enabled by default in both applications.
Fluent mesh export may fail if you are using shared licensing, no licenses are available, and Ansys Fluent is running already. In such cases, the error is due to shared licensing restrictions, but the error message that is issued does not identify licensing as the cause.
For additional information about importing files into Ansys Fluent or Ansys Fluent Meshing, refer to the documentation available under the Help menu within the respective product.