CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   STAR-CCM+ (http://www.cfd-online.com/Forums/star-ccm/)
-   -   Hypersonic flow setup (http://www.cfd-online.com/Forums/star-ccm/87315-hypersonic-flow-setup.html)

screech1987 April 17, 2011 08:57

Hypersonic flow setup
 
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

f-w April 18, 2011 12:26

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

screech1987 April 19, 2011 06:21

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 April 19, 2011 08:10

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?

f-w April 19, 2011 12:49

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 ...

screech1987 April 22, 2011 12:44

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 April 27, 2011 15:00

1 Attachment(s)
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.


All times are GMT -4. The time now is 05:41.