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

Fluent and supersonic flows with strong shock waves

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 15, 2011, 08:50
Default Fluent and supersonic flows with strong shock waves
  #1
New Member
 
Georgy
Join Date: Apr 2011
Location: Russia
Posts: 19
Rep Power: 6
gera is on a distinguished road
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 is offline   Reply With Quote

Old   October 24, 2011, 13:21
Default
  #2
Member
 
navid
Join Date: Jan 2010
Posts: 89
Rep Power: 7
ndabir is on a distinguished road
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.
ndabir is offline   Reply With Quote

Old   October 25, 2011, 00:29
Default
  #3
New Member
 
Georgy
Join Date: Apr 2011
Location: Russia
Posts: 19
Rep Power: 6
gera is on a distinguished road
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
Attached Images
File Type: png Plate.png (8.5 KB, 292 views)
gera is offline   Reply With Quote

Old   October 29, 2011, 13:51
Default
  #4
Member
 
navid
Join Date: Jan 2010
Posts: 89
Rep Power: 7
ndabir is on a distinguished road
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 is offline   Reply With Quote

Old   October 31, 2011, 00:45
Default
  #5
New Member
 
Georgy
Join Date: Apr 2011
Location: Russia
Posts: 19
Rep Power: 6
gera is on a distinguished road
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
gera is offline   Reply With Quote

Old   December 15, 2011, 05:35
Default
  #6
New Member
 
qingkai
Join Date: Apr 2011
Posts: 11
Rep Power: 6
sailor is on a distinguished road
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 View Post
Hi everybody!

I'm trying to carry out simulation for strong shocks (2d or 3d, it doesn't matter).
sailor is offline   Reply With Quote

Old   December 15, 2011, 06:21
Default bug
  #7
Member
 
karthickeyan
Join Date: Feb 2010
Location: coimbatore
Posts: 36
Rep Power: 7
karthickeyan is on a distinguished road
Send a message via Skype™ to karthickeyan
hi there is bug in fluent 6.3 using fluent 13.0 it is possible


Quote:
Originally Posted by gera View Post
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.
karthickeyan is offline   Reply With Quote

Old   December 15, 2011, 23:44
Default
  #8
New Member
 
Georgy
Join Date: Apr 2011
Location: Russia
Posts: 19
Rep Power: 6
gera is on a distinguished road
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 is offline   Reply With Quote

Old   December 16, 2011, 01:14
Default
  #9
New Member
 
qingkai
Join Date: Apr 2011
Posts: 11
Rep Power: 6
sailor is on a distinguished road
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 View Post
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 is offline   Reply With Quote

Old   December 16, 2011, 05:28
Default
  #10
New Member
 
Georgy
Join Date: Apr 2011
Location: Russia
Posts: 19
Rep Power: 6
gera is on a distinguished road
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.
gera is offline   Reply With Quote

Old   April 10, 2014, 14:34
Default
  #11
New Member
 
Chandrasekhar
Join Date: Oct 2013
Location: new jersey
Posts: 24
Rep Power: 3
chandrasekhar is on a distinguished road
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 View Post
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?
chandrasekhar is offline   Reply With Quote

Old   April 12, 2014, 09:50
Default
  #12
Member
 
navid
Join Date: Jan 2010
Posts: 89
Rep Power: 7
ndabir is on a distinguished road
Are you running your case using double precision? Cause if I remember correctly my problem was I did not use double precision.
ndabir is offline   Reply With Quote

Old   April 21, 2014, 02:16
Default
  #13
New Member
 
christina
Join Date: Jul 2013
Posts: 2
Rep Power: 0
christina1990 is on a distinguished road
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
christina1990 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
Assistance for modelling unsteady supersonic flow in FLUENT SATISH A.V FLUENT 11 October 1, 2014 22:36
strong shock solutions Ershath FLUENT 0 November 30, 2010 09:29
Do Fluent can predict shock in supersonic flow? padmanathan FLUENT 0 November 2, 2010 00:11
Shock Reflections in Fluent Richard FLUENT 2 September 2, 2004 09:55
Supersonic Jet Flows Danny Tan FLUENT 0 November 30, 2001 22:01


All times are GMT -4. The time now is 22:44.