CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Main CFD Forum (http://www.cfd-online.com/Forums/main/)
-   -   Hypersonic flow over a re entry capsule with spike (http://www.cfd-online.com/Forums/main/114547-hypersonic-flow-over-re-entry-capsule-spike.html)

navu March 13, 2013 05:36

Hypersonic flow over a re entry capsule with spike
 
Hello,

I am trying to set up the steady, axi-symmetric flow over a re entry capsule with an aero-spike attached at its front. I have played around with a variety of domains and mesh sizes and almost always, it fails to converge when I run the case in fluent. I have given Mach no = 6 and free stream pressure and temp of 1064 Pa and 234k resp. I gave pressure far field for my inlet and top and pressure outlet at the right outlet. The capsule plus the spike was assigned as wall. I have used a variety of solvers, including k-e, k-w and k-w sst models. I also tried varying the CFL number and the implicit and explicit formulation but regardless, I get oscillating residuals which fails to converge. I am really stuck up and any ideas/suggestions/advice would be appreciated.
thanks :)

flotus1 March 13, 2013 06:03

Typical suggestions would be
  • assume inviscid flow
  • ramp up the Mach number
  • instead a rectangular domain with three different boundary faces, use a half-circular domain with only one boundary face and apply the free-stream BC to this face

meshwarrior March 13, 2013 08:11

Such a flow often reveals phisycal unsteadiness depending mainly on the form of capsule head.
For example http://www.cfd4aircraft.com/Publicat...AIAA_J_DF1.pdf.
Inviscid and viscid flows will be qualitatively different in this case.

navu March 13, 2013 13:36

Thanks for the quick reply guys...

And as for your suggestions,

1. I have already tried inviscid, and it immediately diverges after abt 100 iterations.

2. I didnt understand what u meant by ramping up the mach no. U want me to further increase beyond mach 6 ?

3. Like u said, my initial setup consisted of a rectangular domain with the body lying on the axis. Now I have changed it to a semi circular curve at the inlet and gave the free stream there. I am running the case in fluent as I speak. Again, I seem to getting straight or slightly oscillatory residuals to start off. (just reached about 2000 iterations). I gave the initial CFL as 0.01 and then increased it by 0.02 for every 500 iterations. I am not sure I am doing it correctly, but just trying something based on what I read somewhere.

flotus1 March 13, 2013 14:02

Quote:

Originally Posted by navu (Post 413752)
2. I didnt understand what u meant by ramping up the mach no. U want me to further increase beyond mach 6 ?

I meant that you start with a low mach number and increase it until you get the Mach number you want.

navu March 13, 2013 15:06

Alright, I will try that too...

meshwarrior March 14, 2013 01:21

Quote:

Originally Posted by flotus1 (Post 413756)
I meant that you start with a low mach number and increase it until you get the Mach number you want.

Do you mean Reynolds number?

flotus1 March 14, 2013 03:09

No, I meant the Mach number. To be more precise, the mach number specified at the free stream boundary condition. Why do you ask?

meshwarrior March 14, 2013 03:47

At lower Re viscosity damps various oscillations and solution converges "easier" while flow pattern changes not much. It is good practise to use lower Re solution as start approximation for higher Re. Varying Mach number significantly changes flow pattern and to my mind different M -> completely different case. Howewer may be with higher M numerical scheme would behave more stable.

flotus1 March 14, 2013 04:01

I didnt say he should decrease the mach number. Of course the flow at Ma=4 is different from the flow at Ma=6.

I meant he should start the simulation at lower Ma and icrease Ma slowly over the iterations.
Of course in the end the mach number has to be the one he wants to simulate.

meshwarrior March 14, 2013 05:36

Sorry for misunderstanding:)

navu March 14, 2013 06:16

I am a bit confused here. What I am trying to do is to find the cd and temperature reduction on the surface of the capsule due to the presence of the aero-spike. Some people at my university are suggesting that I don't need converged solution necessarily, and its enough if I run about 50k iterations and see if the flow has developed properly. U guys think that would be enough?

meshwarrior March 15, 2013 01:29

You can make fluent show not only residuals but Cd versus time. If you got Cd stabilized or oscillating periodically then you can stop calculation. Likewise temperature at some control points.

navu March 15, 2013 13:15

Yes that's exactly what I am getting. Oscillating cd values versus time. My question is can I stop the iterations now and take the results ?

meshwarrior March 15, 2013 13:50

I'd stop if amplitude and period remains constant with time during Diameter/Uinfinity.

navu March 16, 2013 01:12

Thanks a lot...I think I seem to have solved the problem now.

meshwarrior March 16, 2013 02:54

Quote:

Originally Posted by navu (Post 414329)
Thanks a lot...I think I seem to have solved the problem now.

Mesh independence tests:)


All times are GMT -4. The time now is 03:19.