CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Meshing & Mesh Conversion (http://www.cfd-online.com/Forums/openfoam-meshing/)
-   -   PointWise and GridGen (http://www.cfd-online.com/Forums/openfoam-meshing/61614-pointwise-gridgen.html)

alexandrepereira June 9, 2008 21:23

Hi Foamers, I was wondering
 
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

egp June 10, 2008 05:03

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

alexandrepereira June 10, 2008 13:00

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

olesen June 11, 2008 03:03

Alex, Maybe the "snappyHexM
 
Alex,

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

alexandrepereira June 12, 2008 09:06

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

olesen June 12, 2008 09:23

Alex, Sorry I have no idea
 
Alex,

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

bastil June 12, 2008 16:43

Hi, I am also looking forwa
 
Hi,

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

Regards.

cnsidero June 18, 2008 15:40

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.

egp June 18, 2008 16:32

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

cnsidero June 18, 2008 17:24

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

dkingsley July 10, 2008 09:56

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.

aerospaceman November 24, 2009 12:09

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.

ziad September 4, 2010 21:09

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

cnsidero September 5, 2010 15:33

Quote:

Originally Posted by ziad (Post 274041)
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

Eren10 June 29, 2011 04:28

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.

aerospaceman June 29, 2011 06:34

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.

ziad June 29, 2011 09:30

Quote:

Originally Posted by Eren10 (Post 314010)
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.

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.

aerospaceman June 30, 2011 22:51

Quote:

Originally Posted by ziad (Post 314064)
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.

ziad July 1, 2011 13:29

Quote:

Originally Posted by aerospaceman (Post 314327)
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.

Eren10 July 7, 2011 10:01

Quote:

Originally Posted by ziad (Post 314064)
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.


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.


All times are GMT -4. The time now is 09:31.