Use COMSOL Multiphysics mesh in OpenFOAM for CFD simulations. This tutorial introduces the export and conversion workflow.

You have a good mesh in COMSOL. Getting it into OpenFOAM takes a few specific export (COMSOL), conversion (Gmsh), and import (OpenFOAM) settings. This post walks through the settings and the conversion that works, there are a few widgets to try with along the way. At the end a link to Python script for automating the Gmsh conversion step is provided.

Overview

OpenFOAM (OF) offers a flexible framework and a wide range of solvers for computational fluid dynamics (CFD). However, preparing geometry, generating a mesh, and configuring a case can take considerable effort particularly when a study requires repeated geometry changes. On the other hand, COMSOL mutliphysics combines integrated CAD design and mesh generation modules with the mutliphysics solvers. For users already working in COMSOL, this offers a convenient way to modify a CAD geometry and regenerate mesh without maintaining a separate geometry and meshing workflow. Moreover, COMSOL is equipped with an automatic mesh generation engine which can generate mesh and facilitates process such as face and boundary layer mesh generation.

Combining the two gives COMSOL users access to OpenFOAM’s dedicated CFD solvers, and gives OpenFOAM users a fast geometry and mesh modification platform. A good quality COMSOL mesh will usually pass the OpenFOAM checkMesh requirements, therefore the mesh generated by COMSOL can be used in OpenFOAM solvers, which is what makes this combination practical.

Workflow at a glance

The conversion has four steps. Each has a few details that matter, discussed below. Click a card to jump to it.

1. Exporting the mesh from COMSOL

Once mesh generation is complete in COMSOL, right-click the Mesh node and select Export. Choose Nastran (.nas) as the file type. Figure 1 shows the export settings for the pitzDaily tutorial mesh generated in COMSOL.

Figure 1. COMSOL export settings for the pitzDaily mesh, showing the Nastran file type, selected data, and second-order element option.

In the Data to export section, select domain elements, boundary elements and geometric entity information. The last one stores the surface or volume number of every element in the file, which is what lets you identify surfaces and volumes and assign them to physical groups in Gmsh. Finally, uncheck Export as second-order elements, so that the file contains first-order elements for the gmshToFoam conversion. Once everything is set, export the .nas file. It is ready for the Gmsh session.

Note: check the boxes below and the checklist shows whether the file will work.

Why does the second-order mesh look like? Toggle the element order to see differences.

2. Converting the mesh to Gmsh

Open the exported .nas file in Gmsh, then:

1. Name the boundaries. Go to Geometry → Physical groups → Add and select Surface. In the physical group window, name each boundary group and assign the corresponding surfaces to it. The physical-group definitions are saved in a .geo file. Note that surfaces left unassigned will appear under defaultFaces after conversion to the OpenFOAM mesh.
2. Name the volumes. Repeat the process with Geometry → Physical groups → Add → Volume, and assign a label to each domain.
3. Mesh module. Under Mesh → Define, select 3D and, if desired, Optimize 3D.
4. Export. Go to File → Export, select Mesh – Gmsh MSH from the drop-down menu, and choose Version 2 ASCII in the export window.

The resulting .msh file can be imported into OpenFOAM with gmshToFoam. Figure 2 shows the Gmsh session, with the physical-group and mesh menus highlighted.

Figure 2. Boundary selection for the pitzDaily mesh in Gmsh, the physical-group and mesh menus are highlighted in the sidebar.

3. Importing the mesh to OpenFOAM

The next step is to convert the .msh file with gmshToFoam. Place the file in the OpenFOAM case directory, which should contain the system and constant folders, and run:

gmshToFoam mesh.msh

Replace mesh.msh with the name of your exported file. The conversion creates the mesh in constant/polyMesh. Afterwards, inspect constant/polyMesh/boundary: the imported patches may carry the generic patch type and need to be changed manually where another type, such as symmetryPlane or empty, is required. Panel below shows common boundary types and corresponding modification plus some relevant information.

Note: Cyclic boundaries need additional preparation. The paired surfaces require identical meshes in COMSOL, followed by patch configuration in OpenFOAM with the createPatch utility and a createPatchDict.

4. Checking the mesh

Run the standard check and visualize the result in ParaView:

checkMesh
touch case.foam   # then open case.foam in ParaView

Compare the cell count with the mesh statistics in COMSOL, and look at the patch names in the boundary file. If something looks off, these are the usual errors:

Automated Gmsh script

Naming surfaces by clicking through the Gmsh GUI can be automated, especially when the geometry changes and you re-export the mesh again. So I wrote a Python tool/script that does the conversion and the naming from the terminal. It:

• converts the .nas mesh to first-order elements and checks that gmshToFoam can read every element type,
• lets you name surfaces and volumes at a prompt, with an optional Gmsh window that shows the surface numbers while you type,
• writes the MSH 2.2 file, reads it back and checks the groups and element counts before putting it in place,
• stores the boundaries and their bounding boxes in a small JSON file, so a re-export of the same model can be done fast (--groups).

View the repository on GitHub

pip install gmsh
python nas_to_msh.py pitzDaily.nas
gmshToFoam pitzDaily_named.msh

Re-exported the mesh with a different element size? Reuse the names:

python nas_to_msh.py pitzDaily.nas --groups pitzDaily_groups.json

The script asks for a group name and the surface numbers that belong to it. Try the naming step here. The pitzDaily mesh has 10 surfaces, and the box below shows what the tool would write into the $PhysicalNames section of the .msh. Prefer to see a whole run first? Step through a complete session below. The mesh sizes and bounding boxes are illustrative values, the output format is the real one.

If you use it, I would be glad to hear how it works on your meshes. Issues and suggestions are welcome in the repository.