Hi everyone,

I am calculating flow field in so complicated meshes which have been generated using pro-star. As the iteration goes on, momentum & turbulence residuals decrease while only mass residual fluctuates and finally diverges. To my experience, FLUENT converges well in many problems. So I hope to run my model with FLUENT. The thing is that I could not translate the current STAR meshes into FLUENT mesh. I tried to save the mesh data on pro-star GUIde but failed to import them in FLUENT. If anybody knows how to do it, please help me.

Export the star mesh in nastran format and import that in fluent. Both read and export nastran format.

I've observed this problem with STAR and it is typically a problem of grid quality, grid size in areas of sharp gradients or near the boundary, or another problem with initialization or set up. The grid should be pretty simple to reproduce within Fluent if you generated it in ProSTAR. If you made the grid in ProAm and it's trimmed cell, it may not be transferable to FLUENT.

Jihwan,

Have you tried reducing the relaxation factor for P.

For complex trimmed meshes .02 is used instead of .3, this could help, although it will take longer for convergence.

Kevin

Many thanks to Carno, Ed, and Kevin. Your comments are so helpful.

1. Of course, I don't use trimmed cell simply because the geometry is so complicated. When I tried to make trimmed mesh, I tried various average mesh size and threshold values but the STAR gives around 100-200 unresolved cells. It is too many for me to handle them. So I decided to use tetrahedral mesh. Anybody have suggestions to reduce unresolved cells?

2. I think the mesh quality is not so good. It is simply because the geometry is so complicated. IGES file size is 40M byte for my geometry of a reactor (3 m in diameter) with lots of internals. Do you know how to check skewness of tetra cells and plot them in window to check where these cells are located?

3. I am using SIMPISO with relaxation factor for P of 0.1. I have never thought of 0.02. Oh my god, it is too small. Currently, single iteration step takes more than 20 minutes with my dual Opteron workstation. Probably, I have to expand my computing environments.

4. I tried to export grids in NASTRAN format. The output windows say warning like "cell # is pyramid. Pyramid cannot be translated. I use tetrahedal cells with sublayer.

hi! here is a better way to do this transfer.I have been success before.

1. Export STAR-CD Grid in STAR-CD FORMAT OR OTHER.

2. Import the mesh into ICEMCFD and change the surface into correct boundary family.

3.export to fluent grid.

ps. If you are already know that you have to solver in different software. You must generation you mesh in 3rd party software.

Hi, I have two methods, 1.write the patran file in star and import directly into fluent. 2.write the domain file in star,Import into ICEMCFD and write the fluent.msh file.

Thanks Dhandapani.

Convert the problem into the new STAR-CCM+ code and run your analysis in the new solver.

Hi,

I have the same problem for convergence during a steady simulation with Comet: at the beginning the solution seems to converge (the residuals decrease), but after a while it begins to oscillate and then to diverge. The problem is quite easy (water flow in a pump from inlet to outlet and no movement of any part of the wall), but not the geometry (although I think that there could be of course more complicated geometries!).

I tried to change many parameters and to use pseudotransient mode and yesterday I tried putting 0.02 the relaxation factor for P. It didn't help the convergence!

Then I think probably the problem is the grid, but I cannot make it finer because of memory (and also other) problems.

Any other suggestions? What about the STAR-CCM+ named by Father Dougal?

Thank you everybody,

Erika