CGNS output problem
 

Hello again,

i am trying to mesh a litle laval nozzle with a unstruct mesh with a thickness of one cell. The goal is to compare the results of a compressible calculation (density based) from fluent with the results of the free cfd solver code saturne. For this reason i have tried to export the mesh to a cgns format, but for any reason the exported cgns mesh cannot be opened. neither in fluent nor in cfx. I have checked the mesh by icem, but it´s allright and when I export the mesh to a fluent or CFX fortmat, the mesh can be opened. I am sticking in the mud and need help to create succesfully a cgns mesh..
hope you can help me!

issues...
 

I think there may be some issue with the 2D CGNS output... Something to do with the upgrade to 3.0 libraries having issues with certain aspects in the earlier versions (such as 2D for CGNS 2.4). I am not exactly sure about all the issues, but development is working thru them.

Does this other program accept any other formats?

Do you have access to any older versions of ICEM CFD? (that don't have the CGNS 3.0 libraries)?

If not, I could quickly translate this for you using an older version, just so you can get going again while we figure out what the issue is.

A fair benchmark would require a better mesh.
 

Just a side issue, but for optimal results in fluent, assuming a viscous wall, you really need better boundary layer distribution and orthogonality... I have never heard of Saturne, but perhaps it would also appreciate the better grid.

This can be done with edge parameters and smoothing...

I recommend a better mesh before concluding your benchmark. Or perhaps the benchmark could include a variety of mesh types and densities.

Hi Simon,

thank you very much for your help. The grid is very coarse, especially in the near of the wall, but i will calculate a inviscid flow without shock and compare it with analytical results. I have calculated the case in fluent with this mesh (fluent v6 output of icem) and it agrees quiet well. Code Saturne also supports I-deas universal files and so i will try to use these output option in icem..

is there anything I should know about this format?

Enclosed:
I have the reason of the poor mesh quality. The grid appears to be localy shifted. I have attached 2 pictures. What can be the reason? The geometry is straight.

Edge distribution
 

Your edge distributions are not well aligned... You could copy the one edge distribution to the other or you could set up periodicity...

Thank you Simon,

with the periodicity the edges are now straight. But I have no idea why they were shifted before. I have built the geometry nearly 10 times by creating one side and copying it in z-direction by the transform - translate tool. Then I have created a 3D block bounding box. I have cut it, I have associated the edges to curves and the vertices to points.. as always, but when I create a pre mesh, the two sides of the mesh are shifted!! That is so frustrating :(

As you have advised me in your post, I have tried to smooth the mesh orthogonal, but if i try to do this, icem crashes with the follow error message:

After a renumbering the smoothing is now possible, but it makes nothing better. Maybe I don´t know how to perform the smoothing. Any tipps or tricks?

And is there any reason why the I-deas mesh works in fluent with all areas but not in cfx? (pic 2)

Does ICEM not support the GAMBIT neutral output?

You can see that the smoother is trying to make things orthogonal and trying to smooth out volume transitions, etc. It is just tough to do with such a coarse mesh... That mesh you showed is still probably better than your original. Remember, individual quality may go down, but the solver is actually more concerned about orthogonality and transition between elements. You could try a lot more iterations, you could fix (Freeze) the initial height on the curving wall... 13.0 works much better than 12.1 and there is also a beta option for structured smoothing that I really prefer.

The ICEM CFD output to ANSYS CFX should work... But once in CFX, you say you are importing from ICEM CFD.

ICEM CFD does not support the Gambit neutral output, but it does output in Fluent v6 *.msh format, and both Fluent and CFX will read that in no problem.

The I-DEAS product (Masters Series) is really out of date. We have almost no customers working in that format and ICEM CFD stopped selling our IDEAS CAD reader years ago. The IDEAS output is still there because there is no pressure to remove it, but it is not receiving much attention. You could submit a defect for the CFX team, but I doubt (just my guess) they would would be too worried about issues with reading the rarely used IDEAS format when you have the option of using the Fluent msh or CFX formats...

Ok.. but i am searching for a compatible format for code saturne and the I-deas mesh does not work with code saturne,too. There is a failure with the mesh while the pre procress is running. When I was working for the german aerospace center, I used GAMBIT with code saturne and it worked very fine. Now with ICEM there seems to be no way to export a mesh to code saturne..

I will send you an email with the mesh in fluent v6 format. Please convert it to cgns 2.4

Is ANSYS 13 already out? What are the innovations? :)

Problem is solved!

ICEM 12.1 has a bug with earlier cgns formats, but with ICEM 11 it is no problem to export a cgns mesh to code saturne. You only have to create default BC patches and use face elements for BC patch.

Thank you for the support Simon!

Just to be clear, the bug was with the CGNS 3.0 libraries we included with 12.1 and 13.0. They have trouble when exporting Hexas in CGNS V2.4 or 2.5. There is some other workaround that can be done to fix the files, but we are working to update the library for the next release. I expect to have a patch sooner or later. Let me know if you need it.

hi, Simon,

The exporting problem about ICEM to CGNS is due to the version of FLUENT?

I met the same problem right now.