Pointwise grid export to Openfoam
 

Hi,

I want to export the mesh generated with the Pointwise to OpenFoam. How should I do this.

There is three options at the export: Grid , Database or CAE.
I have only generated mesh, after this only the export > Grid is available. I do not see the right export extensions, even for Fluent.

You will have to build your volume grids in Pointwise and add boundary conditions to the faces before you can export to OpenFOAM using the CAE option.

Dennis

@Eren10

I will add to dkingsley's post.

First, be sure to set you CAE type to OpenFOAM (CAE > Select Solver ... OpenFOAM).

Next, like dkingsley said, you have to have a volume mesh complete. As you know OpenFOAM works in 3D all the time so even if you are doing a 2D simulation you must make the grid 3D first.

Then you can set volume conditions on the volume mesh and boundary conditions on the domains.

Once the above steps have been complete, to save you mesh in the native OpenFOAM format, choose File > Export > CAE ... and the choose the folder to save the files.

For your reference, exporting to Grid allows you to save the mesh only in various neutral or generic formats (PLOT3D, NASTRAN, etc) but no volume or boundary conditions. Export to Database allows you to save the geometry only to various neutral or generic formats (DBA, IGES). The last one, Export to CAE allows to save the mesh, the volume and the boundary conditions to the solver you have chosen.

Hope that helps.

Befor you can export the mesh you have to select all blocks. Then you can export your Volume-Mesh with File -> Export to CAE.

Best regards

Lodda

Thank you guys. I have done it. Also it is important for 2D to generate the third dimension only with 1 step.

Pointwise - OpenFOAM
 

I am new with this Pointwise - OpenFOAM interface, but the issues discussed in this thread are well known to me and already overcome. However I am getting very bad results in OpenFOAM and the settings don't look too bad, so I keep questioning the grid generation... Setting the Boundary Conditions (BCs) is pretty straightforward, but when I set Volume Conditions (VCs) I doubt: should I give a specific name so OpenFOAM recognises it?
My case is quite simple and I only have 1 volume which should be fluid (air), so setting all blocks of the mesh as "set" (which is the only option pointwise offers) is the only thing I can do... so how and where does OpenFOAM read these VCs?
Thanks

You mention building volume condtions. When I tried to this there were no changes to the outputfiles compared to when I only specified bounarys.

How do you specify volume conditions on pointwise and what should the resulting output files looklike?

Thanks

Toby

Dear tobyB,

As far as I have used Pointwise, when exporting to OpenFOAM, it doesn't make any difference whether you specify volume conditions or not. I do not know if it has an implication I might not be aware of, but for how OpenFOAM read the files, specifying volume conditions is not necessary. If you are exporting into OpenFOAM you should get 5 files named boundary, faces, neighbour, owner and points.

Hope this helps,

MDB

Ah okay then, do you know then how I would use those files in order to define different regions?

I am working of the example: chtMultiRegionSimpleFoam->multiRegionHeater. Which seems to define different regions by using boxToCell and then setToCellZone, highlighting cells within a cuboid shape. Although this is fine for simple examples, I need to define more complex geometries to a specific region.

Would this be possible using some of the boundary conditions that you can export from pointwise, and then using faces to select the cells.
Or should I perhaps export the mesh twice, selecting each block section seperatley, two get two sets of boundary points etc? If so, how would I connect these up?

Thanks,

Toby

As MDB said, setting volume conditions for OpenFOAM export does nothing.

right then, so what do you think the best way of implemeting different cellzones from pointwise meshes would be?

Actually, I spoke too quickly. I forgot the ability to export volume conditions as cellZones and cellSets was recently added to Pointwise OpenFOAM exporter. If you grab the latest release candidate, it has this capability:

http://www.pointwise.com/support/dload_rc.shtml

What the volume condition writes out is controlled by the solver attributes found in CAE, Set Solver Attributes.

-Chris

which version are you talking about specifically?
I just got 17.1 R3, does it have to be C4 too? If this works then it will be a great help.

Ok, ive only tried it briefly but the new version (not just R4) did give me some good results. Ill try tommorow to encorperate them into an existing case. Thanks alot cnsidero.

Toby

Hello.
If you have older version of Pointwise you will not be able to export face and cell sets directly as openFOAM mesh file. Workaround is to export mesh as ANSYS FLUENT and then use fluent3DMeshToFoam to convert it to openFOAM mesh.
Then you will have all cell and face sets.

Update on the solution (2019)
 

I've been struggling with Pointwise + OpenFoam, but I figure out something that make all the difference:

1. when extruding the mesh in Pointwise (in the z-direction, for example), select: translate -> assemble: ONE-FACE-PER DOMAIN -> verify if it is really selecting ONE face per domain.

2. in OpenFoam, use: renumberMesh -overwrite

also, don't forget to set up the BC and all the other stuff people have already written in here. My solution is converging really quickly now!

Hope this helps someone (and sorry for the bad English!)

;)