CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > STAR-CCM+

Hypersonic flow setup

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 17, 2011, 09:57
Default Hypersonic flow setup
  #1
New Member
 
Martin
Join Date: Nov 2010
Posts: 23
Rep Power: 5
screech1987 is on a distinguished road
Hello,

I was wondering whether anyone has had experience using starccm+ for Hypersonic flow conditions.

I am currently modelling the reentry capsule for a martian probe as part of a uni project. The 3D domain consists of a halfbody of the RV, a symmetry plane and freestream. However when run the AMG solver diverges before 100 iterations, even when fiddling around with courant numbers and relaxation factors and allowable values etc.

I am using the k-w SST model and real gas (CO2 and Redlich-Kwong gas model). I assume my problem is coming from the high speed (M=13!) and low ambient temperature of 163.9K. Also the fact my freestream, is only one boundary, so in reality the boundary conditions spanning over the freestream would change drastically.

Anyway, has anyone ever used Star at such a high Mach number regime sucessfully? Or any pointers to make it run successfully. Thinking about knocking a 2D structured mesh with stupid refinement to be sure.

Cheers
screech1987 is offline   Reply With Quote

Old   April 18, 2011, 13:26
Default
  #2
f-w
Senior Member
 
Join Date: Apr 2009
Posts: 129
Rep Power: 7
f-w is on a distinguished road
I haven't simulated any hypersonic flow, but looking forward to it. Below is a link to a presentation by a Star-CCM+ user on simulating Mach 6 flow which you might find useful:

http://www.cd-adapco.com/pdfs/presen...co-clement.pdf
f-w is offline   Reply With Quote

Old   April 19, 2011, 07:21
Default
  #3
New Member
 
Martin
Join Date: Nov 2010
Posts: 23
Rep Power: 5
screech1987 is on a distinguished road
Well my original setup was the same as what was recorded in the presentation for in terms of coupled flow setup. Except for the inclusion of real gas (as the temperature should be high enough for chemical reactance of the CO2) rather than ideal, and the use of structured meshes.

Tried Explicit integration to see if that helped, which resulted in a longer time to reach divegence in the AMG solver, but divergence all the same.
When I used my high refinementn 2D structured mesh, problems were still encountered under the conditions I set out to model. (under normal atmospheric conditions at mach = 1 the shock was captured with very good definintion)

But will keep fiddling
screech1987 is offline   Reply With Quote

Old   April 19, 2011, 09:10
Default
  #4
New Member
 
Martin
Join Date: Nov 2010
Posts: 23
Rep Power: 5
screech1987 is on a distinguished road
Had a search for 'hypersonic' in the StarCCM+ UG, and found the foolwing recomendations for extreme hypersonic cases using Imlicit Discretization:

-Courant Number ~0.1 (for start up)
-Explicit Under Relaxation Factor 0.75
-Positivity Rate Limit of 0.05

Got up to 1000 iterations (and counting) with this setup, but limitations in cells are still present and residuals are no where near converged. The shock is starting to detach from the aeroshell slowly, which I assume will be the cause of the fluctuating residuals as it moves.

I know the Courant number will need to be raised at some point, but unsure when?
screech1987 is offline   Reply With Quote

Old   April 19, 2011, 13:49
Default
  #5
f-w
Senior Member
 
Join Date: Apr 2009
Posts: 129
Rep Power: 7
f-w is on a distinguished road
Here are a couple of suggestions (don't forget the help file for more info); some of these were introduced in v4.06:

- improve your mesh quality
- cell quality remediation (the lazy, expensive approach to above)
- expert solution driver (will do your relaxation factors and CFL stepping for you)
- while you're at it, try the expert initialization as well (grid sequencing)
- if grid sequencing doesn't help try running the coupled solver with 1st-order discretization for first few hundred iterations
- try using the AUSM+ scheme (instead of Roe)
- you mentioned concern over your freestream boundary, you should enlarge it to be at least of diameter that is 20 times your spacecraft's largest length scale

Keep us posted ...
f-w is offline   Reply With Quote

Old   April 22, 2011, 13:44
Default
  #6
New Member
 
Martin
Join Date: Nov 2010
Posts: 23
Rep Power: 5
screech1987 is on a distinguished road
Well the AUSM+ and grid initialisation seem to have worked a treat. running both 2D with this setup, with what seem reasonable results so far, even if residuals (for 2D) are a little skew wiff, and possibly too higher temperatures in the wake region. However I have a 3D case running with the same setup which seems to be going okay.

Will post back on the final when i have the final outputs.
screech1987 is offline   Reply With Quote

Old   April 27, 2011, 16:00
Default
  #7
New Member
 
Martin
Join Date: Nov 2010
Posts: 23
Rep Power: 5
screech1987 is on a distinguished road
Attached is a bit of a gratuitous scalar scene of the 3D simulation. With Contours of temperature on the Aeroshell body and an Iso-suface at M=13.45
Also the background image was taken from www.dailygalaxy.com.

Still however the simulation has not reached any 'convergence' I feel, so see what will happens after a few thousand more iterations. Of interest/worry is the surface temperatures on the rear of the aeroshell and the wake eminating from it are ~500K in some areas more than on the front heat shield. But probably just a combination of hypersonic condtions and convergence I feel.
Attached Images
File Type: jpg aeroshell_v3@40000_Scalar Scene 1.jpg (27.2 KB, 30 views)
screech1987 is offline   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
Finite Rate Chemistry Setup for Hypersonic Flow AdeeMij FLUENT 8 April 7, 2014 16:45
Channel flow setup in Large-eddy simulation Weihua Main CFD Forum 5 January 24, 2012 06:16
Hypersonic flow scramjet ishaninair OpenFOAM Running, Solving & CFD 0 March 10, 2011 08:45
OpenFOAM case setup and work flow - what are you using? Arnoldinho OpenFOAM Pre-Processing 4 July 18, 2010 10:16
Multigrid for hypersonic flow Jeff Main CFD Forum 0 October 20, 2002 21:50


All times are GMT -4. The time now is 06:34.