PointWise and GridGen
 

Hi Foamers,

I was wondering if anyone ever used/tried PointWise or GridGen as a mesh generator for OpenFOAM?

Is its export format compatible with mesh conversion utilities of OpenFOAM...?

Do the meshes built with these mehers have good qualities for CFD use...? ( skewness, condition, non -orthogonality...)

Thanks in advance

Alex

Hi Alex, We heavily use Gri
 

Hi Alex,

We heavily use Gridgen and Pointwise for CFD analysis at Penn State, and I know of many organizations that use it here in the U.S. Personally, I have used it for 15 years. It's origin is based on algebraic and elliptic methods for structured hex meshes, however, it has capability for unstructured meshing as well.

Since it is a man-in-the-loop type software, mesh quality is related to user experience and expertise. However, as I already said, it is our primary work-horse and allows us to grid very complex systems with acceptable grid quality. For these kind of problems, we do use overset-capable flow solvers which eliminate some gridding constraints, and generally improve grid quality.

Currently, I export the mesh as either FLUENT or STAR-CD, and convert use OpenFOAM converters. This is not perfect, especially for geometries that have pole singularities, or rotationally-periodic (cyclic in OpenFOAMese) patches.

I recently inquired about the addition of direct OpenFOAM export, and was told that it depends upon their business assessment after attending the Milan Workshop. I've heard that they are sending their technical sales engineer.

Also, it would certainly help speed up the process if currently gridgen and openfoam users would submit a request to GRIDGEN for the capability to write native OpenFOAM files.

Eric

Hi Eric Thanks a lot for th
 

Hi Eric

Thanks a lot for this information.

I have used, as a demo, Harpoon Mesher, my trial period is over. Since I am planning to use OpenFOAM as a tool in my PhD studies at Univ. Coimbra in Portugal, I made this question just to figure out what is the best "bang for buck" in meshing software.

The speed of meshing in Harpoon is quite impressive, but as for the mesh quality... some of the meshes ( in the 4 Mil tets size ) did not pass the checkMesh test.

Since my work in PhD will focus on sea keeping qualities of high speed large naval vessels, i guess tha robust meshes as quite essential.

Thanks once more

Alex

Alex, Maybe the "snappyHexM
 

Alex,

Maybe the "snappyHexMesh" in the upcoming version 1.5 will be useful for you.

Hi Mark, I'd love to try it
 

Hi Mark,

I'd love to try it...

In the mean time i have started to test and run the tutorials of Pointwise... seems powerful software...

By any chance could you tell me when will OF 1.5 be available...?

I know beta testing has already started...

Thanks

Alex

Alex, Sorry I have no idea
 

Alex,

Sorry I have no idea how the beta testing and/or release schedule looks.

Hi, I am also looking forwa
 

Hi,

I am also looking forward to test snappyhexmesh. This will be a important step for OF.

Regards.

Since I am the one attending a
 

Since I am the one attending and presenting at the workshop, I thought I would chime in.

Thanks for the initial reply Eric.

To follow up Eric's comment about OpenFOAM export additions, he is not the only one. Particularly since the beginning of this calendar year we have been receiving an increasing number of requests from new and current customers with regards to using our softwares - Pointwise and Gridgen - with OpenFOAM. The high interest in OpenFOAM, coming not only from the academic but also from the commercial community, is the reason for our attendance at the workshop.

Due to a lack of sophisticated meshing tools in OpenFOAM, I felt this would be a good opportunity to reach out to the open-source CFD community and establish a relationship.

As Eric stated, currently the easiest way to get our meshes into OpenFOAM is with one of the formats the translators support, e.g. Fluent. I was not aware of the pole and periodic issues - so thank you Eric. Would you care to expand on that more?

If you haven't seen the session titles/abstracts my presentation is, in a few words, about how Gridgen handles CAD import and cleanup. This currently is one the most troublesome areas of pre-processing so we have developed capabilities to tackle it from two directions: 1) deal with the CAD you are given 2) fix and create watertight geometry. In fact, you can use a combination of two if desired. While that may sound general, I was instructed that the workshop is quite technical and the attendees would be expecting such so I will be presenting a very detailed look into how both of these capabilities work.

Kind regards, Chris

Chris Sideroff, PhD
Technical Sales Engineer
Pointwise, Inc.

Hi Chris, Concerning pole
 

Hi Chris,

Concerning pole singularities, or degenerate surfaces, the problem is with Gridgen's fluent exporter. It simply will not write out the grid. Unfortunately, it is somewhat problem specific. It has worked for some cases, and not others. Most recently, I ran into this problem when generating a grid for the SUBOFF hull form. As a work-around, I wrote the grid out as a STAR-CD format. Is there a check for minimum cell volume that might be causing the problem?

Concerning translational or rotational periodicity (or cyclic b.c.'s in OpenFOAMese), OpenFOAM ultimately wants these boundaries to be identified as a single patch, with each face in the exactly the same order, one after the other. There are tools for coupling the patches (createPatch), and for reordering the patches (couplePatch), but we've really struggled, especially with turbomachinery grids. Currently, when you create cyclic domains in gridgen, it writes out the parent and the shadow as separate patches. It would be a big help if gridgen wrote all of the files to be compliant with OpenFOAM solvers so that we didn't have to deal with this problem.

Eric

Eric, To answer your first,
 

Eric,

To answer your first, since this has to do with Gridgen and you're a customer it would best be answered by call/emailing our support group with the details.

The second is related to how OpenFOAM handles periodic boundaries and may be something that would need to be included should a translator from our format to OpenFOAM ever materialize. Furthermore, because many other codes support multiple domains (i.e. patches) for a single boundary (even periodic), I suspect this would not be changed internally. Perhaps it would be more beneficial to extend OpenFOAM to allow for multiple patches on periodic boundaries. I will qualify this by saying these are strictly my thoughts and haven't consulted with anyone here about it so consider it my opinion and not Pointwise's.

Chris

Eric, I am also having an
 

Eric,

I am also having an issue with poles buried in block faces and using the Fluent export in Griidgen.

I have just sent an email to Gridgen support with details.

Caro Alexandre,

I have seen that you were pondering to use Harpoon and also Gridgen?Pointwise for your PHD in Coimbra.

I have both extensively for my undergraduate studies.

Unfortunately they are not compatible with each other. Gridgen is a highly user intensive program that really requires experience to get a good grid out off. Nevertheless you will get a good grid eventually.

Harpoon on the other hand, is a totally different program. It will give you a mesh in seconds for any geometry. You can put in the CAD for a tree and it will give you a mesh in seconds.

However, you can forget that the Boundary Layer exists in Harpoon. It is highly skewed, irregular and ultimately useless.

So consider wisely if you want to touch Harpoon. For my work, which is more intensive on the flow physics I need to resolve the boundary layer, so harpoon is no good at all. If on the other hand ou want to optimize a Race Car component, harpoon is good because it will show you the trends you need in little time.

Anyway, this was my experience.
Hope this helps.

Highly recommend Pointwise to create OpenFOAM meshes
 

I've been using Gridgen and Pointwise for over three years and recommend both. For about a year now you can export Pointwise meshes directly in OpenFOAM format. Never had a problem with any mesh created with these two packages. Just make sure you run the GridGen/Pointwise own mesh improvement algorithms first and you will get high quality meshes.

Both are fairly easy to learn through the provided tutorials. Gridgen has a lot of very advanced (and poorly documented) features that allow you to micro-manage almost any aspect of the mesh but I've never had to use them. The basic aspects covered in the tutorial make it possible to create quality meshes for both commercial work and research.

Ziad

Ziad, thanks for the nice comments. Would you care to expand on the poorly documented features? If you feel like this, I'm sure there are other people feeling the same way and we would like to address it.

You also may want to write a detailed reply to our support group as they handle the documentation for the software.

Thanks, Chris

Is it possible to generate multi block meshes with Pointwise. I want to vary the distance to the adjacent cell from the airfoil to get the correct y+ distribution.

Yes, it is possible to generate multi-block grids in Pointwise.

Yes, you can most definitively vary the height of the first cell in order to get the Y+ you desire.

Just might add that in doing so you will probably get high aspect ratios on these cells. From my experience, the maximum value should not go above 1000.

Hope this helps.

It depends what you mean with multiblock. The basic approach in Pointwise/GridGen is the divide the computational space in blocks that are meshed separately. These blocks will match perfectly at their common interfaces.

The other concept of producing overlapping, non-matching multiblock meshes is not possible, at least with the version we have. You could still click the mesher into doing it by producing each block independently and sorting out the interfaces in your CFD solver.

Good point. I only ever heard of the first definition of multiblock. Can't quite imagine what benefit of overlapping and non-matching multiblocks can bring. But you live and learn, I guess!
Thanks for that.

Well, strictly speaking non-matching overlapping blocks would constitute an overset grid, or chimera. But put aside the interpolation procedure in the common fringe regions the method is not unlike multiblock meshing. Check out Overture from Lawrence Livermore for examples. https://computation.llnl.gov/casc/Ov...mentation.html

The main benefit is in having structured meshes on geometries that otherwise can not be meshed with traditional single/multi-block method.

I want to define more segments around an airfoil, to have more control over the yPlus values. So, I should create mesh around segment 1 and then go to the segment2 , and pray that the intersection will be oke :D
Doing something with the overlapping region with the Openfoam would be difficult for me. Than I should keep it like it is now.

Eren10 can you post of picture of what you're trying to do to help me understand? I might be better able to give you proper guidance this way.

Thanks, Chris

I have attached a view of what I was trying to do. You can see that there are 2 domains, with overlapping region. This domains should fit at that section.

Eren10 to get the extrusions to match you need to extrude from all the airfoil connectors simultaneously. To do so, select all the airfoil connectors then perform the extrusion (Create > Extrude > Normal ...).

You may need to take some precautions near the trailing edge but I can't see the detail there. Is it blunt or sharp?

It is sharp. I have created a lot of meshes with the method u said. but this way I have not much control over yplus values, but it is oke.

If it is possible I would save the BoundaryConditions once, else I have to type it again, I am using the geometry for different simulations.

And a last question: Is there a general function that will improve the meshquality after the mesh is generated ?

You can still have very good control over the Y+ values by doing it the way Chris advised. It is better to use several connectors on the pressure and suction sides, and then extrude from them all simultaneously. Your mesh will be much smoother and will not overlap.

As for mesh quality tools, you can use the elliptic solvers that come with the structured blocking tools. The default settings should be pretty good for this.

If you run into problems at the trailing edge, build a connector there that is approximately normal to the two surfaces of the airfoil and then extrude along this connector normal to the airfoil surface. Once done, you can then extrude this connector downstream to create your wake region.

It's not clear to me what you trying to accomplish - I am sorry for that. From the picture you attached it looked like you creating an extrusion for each connector ... ahhh, I know what you are trying to do now. You want the near wall spacing to vary along the length of the airfoil.

As you've found out, you can only specify one delta_s when creating an extrusion but there is a way to achieve what you're looking for. First, split the airfoil surfaces at one or more locations, e.g. 50% chord. I see you've done it on the suction side so do the same on the pressure side.

Now create the extrusion with all the connectors. So select them all then Create > Extrude > Normal ... You should now see the Assemble panel. Before clicking Done, in the Assemble Special frame, click Delete All Edges, change the Assemble Type to One Edge Per Connector, click Assemble and then click Done. Perform the extrusion as previously.

You'll notice now that one domain will be created from each connector and there are connectors emanating from the split points in the middle of the airfoil. Using Grid > Distribute you can modify the end spacing and distribution on these connectors to achieve the spacing you want at each location. For example, when I tried it I found that when I modified the spacing I had to also change the distribution function of the connector to Geometric.

The tricky part in the doing the above is that its most likely going to disturb the internal grid lines created the hyperbolic extrusion. You can remedy this by running the domains in the elliptic solver. Pick the domains, Grid > Solve ... and run the solver for 20-30 iterations.

I went through this procedure myself on a NACA4412 with C = 1. I split the airfoil at ~40% on top and bottom. I created a One Edge Per Connector extrusion (as outlined above) with ds = 0.0001, GR = 1.2 and 30 layers. I then change the middle normal connectors wall spacing to 0.0004 and distribution to Geometric. I did the same for the normal connectors at the trailing edge but with ds = 0.0008. I then ran the domains through elliptic solver for 30 iterations with default settings.

See the result in the attached image. It's a bit tough to see but you can make out the expanding BL near the TE.

Let me know how it goes, Chris

Sorry Ziad, you replied before I could finish my long explanation ;-). Thanks for your help.

Don't worry about it :)

BTW I don't think it is necessary to have such tight control over the normal spacing to the wall to achieve a good Y+. If Eren is using RANS with the usual wall function recipes he will need to have 30 <= Y+ <= 150 and this will give a comfortable margin of wall spacing to use.

Another way of doing this would be creating one connector at the TE and then extruding it along the pressure and suction sides, followed with a healthy elliptic solver dose...

To vary the yPlus values I should be able to change the y distance to the first cell. With the procedure you explained this can't.

I am trying to reduce simulation error as far as I can. Anyway, I will continue with the one normal extruded mesh.

Thank you Chris and Ziad.

I have a question about the function " solve " in Pointwise. I think this can be done after mesh is generated. Wat is its function ? Shall the mesh quality improve ?

Regards.

Export from pointwise for OpenFOAM
 

Dear Ziad,
You have mentioned that it is possible to export Pointwise meshes directly in OpenFOAM format. Before I begin creating the mesh in Pointwise, I can choose OpenFOAM as the solver. After creating the mesh, it is possible to export it as a grid file (.gg). Would you please let me know what further steps should be taken to generate the mesh in OpenFOAM, by using this .gg file?

Hi,

Not sure I understand what you mean. I haven't used Pointwise for a while now and don't have a license available for checking, but off the top of my head *.gg is the original GridGen format. Why do you need it anyway? Save your mesh under pointwise format (*.pw) and proceed as usual. The manual has all the info needed.

Ziad

Thanks for your response. To make my question clear, as you know, it is possible to convert a mesh created in a commercial software, into the format that OpenFOAM uses. For exam, "gambitToFoam" command is used for converting a gambit mesh to OpenFOAM format. My question is that, what is the process to convert the ".pw" file to the format that OpenFOAM uses.
Thanks in advance!

Pointwise has native export into OpenFOAM format. No need to use an OpenFOAM utility, an there isn't one anyway. Just go to Export->CAE under the File menu in Pointwise. For details check the manual.