CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CD-adapco

How to convert STAR mesh into FLUENT mesh ?

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   November 8, 2004, 03:44
Default How to convert STAR mesh into FLUENT mesh ?
  #1
Jihwan
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   November 8, 2004, 09:09
Default Re: How to convert STAR mesh into FLUENT mesh ?
  #2
carno
Guest
 
Posts: n/a
Export the star mesh in nastran format and import that in fluent. Both read and export nastran format.
  Reply With Quote

Old   November 8, 2004, 19:16
Default Re: How to convert STAR mesh into FLUENT mesh ?
  #3
Ed
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   November 8, 2004, 19:25
Default Re: How to convert STAR mesh into FLUENT mesh ?
  #4
Kevin
Guest
 
Posts: n/a
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
  Reply With Quote

Old   November 8, 2004, 19:47
Default Re: How to convert STAR mesh into FLUENT mesh ?
  #5
Jihwan
Guest
 
Posts: n/a
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.

  Reply With Quote

Old   November 9, 2004, 04:01
Default Re: How to convert STAR mesh into FLUENT mesh ?
  #6
tomosada
Guest
 
Posts: n/a
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.

  Reply With Quote

Old   November 9, 2004, 09:47
Default Re: How to convert STAR mesh into FLUENT mesh ?
  #7
Dhandapani.s
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   November 10, 2004, 00:45
Default Re: How to convert STAR mesh into FLUENT mesh ?
  #8
Father Dougal
Guest
 
Posts: n/a
Convert the problem into the new STAR-CCM+ code and run your analysis in the new solver.
  Reply With Quote

Old   November 10, 2004, 04:11
Default Re: How to convert STAR mesh into FLUENT mesh
  #9
Erika
Guest
 
Posts: n/a
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
  Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
How to convert OF141 mesh to OF13 mesh hsieh OpenFOAM Meshing & Mesh Conversion 3 June 22, 2009 09:31
How to convert a hex mesh in blockMeshDict to a tet mesh henning OpenFOAM Running, Solving & CFD 1 October 14, 2008 07:02
convert star files to fluent (couples) azmir FLUENT 6 May 6, 2004 04:56
Convert FLUENT mesh to some other format for STAR? Jiaying Xu FLUENT 3 December 5, 2002 08:15
convert FLUENT mesh file to CFX mesh file?? frederic felten FLUENT 5 December 6, 1999 09:32


All times are GMT -4. The time now is 02:03.