CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Fluent and supersonic flows with strong shock waves (http://www.cfd-online.com/Forums/fluent/87264-fluent-supersonic-flows-strong-shock-waves.html)

gera April 15, 2011 08:50

Fluent and supersonic flows with strong shock waves
 
Hi everybody!

I'm trying to carry out simulation for strong shocks (2d or 3d, it doesn't matter).

I've always got the same problem: temperature limited to 1.000000e+00 in 11 cells on zone 2... and so on.

I tried to use Fluent 6, 12, 13. Everything looks not good.

I have found that:
1. 1st order upwind scheme is very safety (no warnings, mentioned above)
2. shock waves are very thick (which is normal, but it is also not good)

So.., the question is - does anybody use Fluent for supersonic flows (M=4-12) with strong shock waves?
How to use high order schemes (2nd upwind or 3rd MUSCL) in Fluent with strong shock?

If somebody had experience with this problem, please, give some comments on it.

Thanks in advance.

ndabir October 24, 2011 13:21

Hi,

I have the same problem. I need to capture shock production because of very high pressure gradients (1 GPa) and I get the same errors that you mentioned even with the first order method. I am using an explicit solver since I could not get convergence with implicit solver.

Have you solved your problem? If yes would you please help me with it.

gera October 25, 2011 00:29

1 Attachment(s)
ndabir,

Yes and no, at the same time!
Currently, I'm using Fluent 12 with 3rd MUSCL and implicit solver for steady case.

As far as I can see, Fluent can calculate some problems with shock waves, but it depends on geometry and particular case.

For example,

Few days ago I tested code for Temperature Jump and Slip Velocity boundary conditions. I solved hypersonic flow around plate and fluent has calculated it fine (see Figure attached). I used 2nd upwind with AUSM solver.

On the other hand, I also tried to calculate 2D ramp (plate with additional flap with angle 27 deg) and Fluent crashed!

General issue that you can try to overcome this problem:

1. Try to reduce CFL (Courant number)
2. Try to resolve boundary layer more precisely - try to draw mesh in to a wall (It is necessary to have Reynolds number based on cell size about unity inside boundary layer, Re~1)
3. Try to use AUSM solver instead of Roe (if you used Roe one)
4. Try to change limits (Solution Controls -> Limits) in Fluent
5. The problem can be at initial time moment, sometimes it is necessary to specify special initial conditions, for instance, to overcome vacuum problem. You can try to initialize flow with a rest gas.
6. Try to reduce inflow pressure to increase influence of physical viscosity (just for test)

What do you try to solve? Steady/unsteady, 2D/3D....

If you get any results (successful or not), please, send you comments here.

All the best,
Gera

ndabir October 29, 2011 13:51

Thanks for your reply gera.

actually I am solving a 2D unsteady shock propagation. There is a very small sphere (bubble) in the middle of domain as pressure inlet near wall and there is a large diameter half circle surrounding it as pressure outlet or far field.

The pressure in inlet is 1 GPa and temperature is 5000 K. The whole domain is in atmospheric conditions.

I will get reasonable results for pressure inlets in the order of 10 MPa, but as I increase the inlet pressure, at the very first steps I will see this error:

"Error: > (greater-than): invalid argument [2]: wrong type [not a number]
Error Object: 1.#qnan

Error: WorkBench Error: Could not handle event: SolutionStatusUpdate
Error Object: #f"


which I think the temperature gradient is very high (I am not sure.)

my mesh is triangular and very fine near the inlet.
I use explicit solver with ASUM flux calculator and first order solver. the time step is around 10^-12.

I also change the limits but still have the problem.

Do you know how can I handle this error?
Is it better if I use pressure-base solver or density-base?

gera October 31, 2011 00:45

ndabir,

Honestly, I have never seen this error before. So, I cannot give you correct/direct solution, but I think you can try following things.

1. Try to reduce pressure, for example in 10^6 times, so you will get 10^3 Pa in inlet and ~1 Pa in domain. (It is necessary just for test. As I understand you have already tried.)
2. Check operating pressure (Boundary conditions-> operating conditions -> operating pressure should be zero for compressible flow with shock waves)

Are you trying to solve viscous or inviscid problem? It looks like inviscid one.
3. Try to include physical viscosity under low pressure conditions (item #1)

I'm not sure..., but I think it is better to use structured grid.

Half year ago, I was in seminar devoted to Ansys Fluent.
Presenter said that in a case of shock waves density-based solver is preferable.

I tested both solvers in inviscid case (steady flow between two symmetrical wedges). Both solvers worked, but pressure-based solver gives very thick shocks and slip surface.
So, I think in your case, it is necessary try both solvers.

Quote:

I will get reasonable results for pressure inlets in the order of 10 MPa
As I understand If pressure inlet is 10 MPa, everything is ok. And you have already obtained good results for 10 MPa. Am I right?

Are you using single or double precision?
I think in this case, double precision is necessary.

If you get any results, please, write it here.

Best regards,
Gera

sailor December 15, 2011 05:35

Hi,
I have a easier question to ask.

I want to simulate the condition that: Mach number is 1.5 with only a plate.
I set the boundary condition as:
pressure inlet condition by Gaugh pressure 101325Pa, 26704Pa;
pressure outlet as 101325Pa;
pressure far field as 101325Pa.
1order upwind, steady case now.

But the residuals are not converged, how should I set the boundary condition?

Quote:

Originally Posted by gera (Post 303768)
Hi everybody!

I'm trying to carry out simulation for strong shocks (2d or 3d, it doesn't matter).


karthickeyan December 15, 2011 06:21

bug
 
hi there is bug in fluent 6.3 using fluent 13.0 it is possible


Quote:

Originally Posted by gera (Post 303768)
Hi everybody!

I'm trying to carry out simulation for strong shocks (2d or 3d, it doesn't matter).

I've always got the same problem: temperature limited to 1.000000e+00 in 11 cells on zone 2... and so on.

I tried to use Fluent 6, 12, 13. Everything looks not good.

I have found that:
1. 1st order upwind scheme is very safety (no warnings, mentioned above)
2. shock waves are very thick (which is normal, but it is also not good)

So.., the question is - does anybody use Fluent for supersonic flows (M=4-12) with strong shock waves?
How to use high order schemes (2nd upwind or 3rd MUSCL) in Fluent with strong shock?

If somebody had experience with this problem, please, give some comments on it.

Thanks in advance.


gera December 15, 2011 23:44

sailor,

Are the residuals constant? Or its always grow? Oscillating?

For supersonic cases, operating pressure must be equal zero.

About pressure outlet. If flow is supersonic across pressure outlet, it works as supersonic outflow. All quantities are interpolated out of a computational domain. So it's not necessary to worry about gauge pressure of pressure outlet.

I didn't catch. Are you using pressure far field or pressure inlet as a supersonic inflow? I'm using pressure far field and it works fine.

Try to test 2order upwind.

sailor December 16, 2011 01:14

Gera, thanks very much!

The residual oscillated for a short time, then grow up quickly and end the simulation.

I learn your opinion about setting pressure-outlet.
I use pressure-inlet as the supersonic inflow, and want to use pressure-far-field for the other part of boundary. What should I focus when I set the pressure-far-field values?

Quote:

Originally Posted by gera (Post 336023)
sailor,

Are the residuals constant? Or its always grow? Oscillating?

For supersonic cases, operating pressure must be equal zero.

About pressure outlet. If flow is supersonic across pressure outlet, it works as supersonic outflow. All quantities are interpolated out of a computational domain. So it's not necessary to worry about gauge pressure of pressure outlet.

I didn't catch. Are you using pressure far field or pressure inlet as a supersonic inflow? I'm using pressure far field and it works fine.

Try to test 2order upwind.


gera December 16, 2011 05:28

sailor,

I had similar residual behavior (oscillation and rapid increase) when I carried out computations for 3d delta-wing. In that time I reduced Courant number and did about 1000 iteration. After that I set Courant number (about 5) back and continued calculation without any problems. Try to do the same.
Further I noticed that spatial resolution near body wall wasn't enough. Cell Reynolds number was too high.

Honestly, I don't know the difference between pressure-inlet and pressure-far-field. I think it should be similar to each other. But I always use pressure-far-field as supersonic inflow because I think it is easier to use. Just set Mach number, temperature, pressure in free stream and go ahead! )

Did you notice any "boiled" regions (after post processing)? Any unphysical features in flowfields?
PS: When I just started to use FLuent, I had some experience like that. Direction of x axis was opposite to direction of a free stream. I saw only "boiled" flow and crashing of Fluent. But I don't remember version of Fluent.

chandrasekhar April 10, 2014 14:34

Hi
i tried reading a scheme file which reads into Ansys Fluent a case file

////(do ((x 2 (+ x 1))) ((> x 2))

(ti-menu-load-string (format #f "/file/read-case \"E:\t_bouyancy1\tb1_all_cases_files\dp0\FFF\Fluen t\tb1_1_~a.cas.gz\"" x))
)////

i have got the same error
////Error: WorkBench Error: Could not handle command Error Object: #f/////

any help on this would be much appreciated. Many thanks for replying



Quote:

Originally Posted by ndabir (Post 329991)
Thanks for your reply gera.

actually I am solving a 2D unsteady shock propagation. There is a very small sphere (bubble) in the middle of domain as pressure inlet near wall and there is a large diameter half circle surrounding it as pressure outlet or far field.

The pressure in inlet is 1 GPa and temperature is 5000 K. The whole domain is in atmospheric conditions.

I will get reasonable results for pressure inlets in the order of 10 MPa, but as I increase the inlet pressure, at the very first steps I will see this error:

"Error: > (greater-than): invalid argument [2]: wrong type [not a number]
Error Object: 1.#qnan

Error: WorkBench Error: Could not handle event: SolutionStatusUpdate
Error Object: #f"


which I think the temperature gradient is very high (I am not sure.)

my mesh is triangular and very fine near the inlet.
I use explicit solver with ASUM flux calculator and first order solver. the time step is around 10^-12.

I also change the limits but still have the problem.

Do you know how can I handle this error?
Is it better if I use pressure-base solver or density-base?


ndabir April 12, 2014 09:50

Are you running your case using double precision? Cause if I remember correctly my problem was I did not use double precision.

christina1990 April 21, 2014 02:16

hi gera......i want to simulate hypersonic(Pstat=2000pa,Tstat=60k,M=6).....boundar y condition is farfield....but not convergence and oscillation.....can you help me ....Fluent can solve this condition or need UDF???

THANKS


All times are GMT -4. The time now is 13:08.