|
[Sponsors] |
January 4, 2013, 13:22 |
Problem with diverging simulation
|
#1 |
Member
Simone
Join Date: Sep 2012
Posts: 95
Rep Power: 14 |
Hi to everyone guys, I really need some help! I'm running a 3D simulation with adjoint NS equations, but the simulation diverges (residuals seems to remain constant but the error explodes). I've heard that these kind of simulations are really sensitive, and so I would like to set up fvSchemes file with the most conservative/linear/first order schemes, in order to see if the problem is with mesh or with the solution.
Which kind of scheme could I use? Any help is really much appreciated. Thanks a lot Simone |
|
January 7, 2013, 06:52 |
|
#2 |
Member
Simone
Join Date: Sep 2012
Posts: 95
Rep Power: 14 |
Any answer please?
|
|
January 7, 2013, 08:31 |
|
#3 |
Senior Member
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,208
Rep Power: 27 |
hi
Use euler method in schemes for more stability.whats the error?give it in code tag. |
|
January 7, 2013, 08:55 |
|
#4 |
Member
Simone
Join Date: Sep 2012
Posts: 95
Rep Power: 14 |
Hi thanks for your answer! My simulation is steady-state, so, where could I use Euler method? I was thinking about upwind method instead; could it be correct?
The error is about the adjoint continuity error, which explodes.. |
|
January 7, 2013, 09:21 |
|
#5 |
Senior Member
Daniele Vicario
Join Date: Mar 2009
Location: Novara, Italy
Posts: 142
Rep Power: 17 |
Maybe this two posts could help you:
http://www.cfd-online.com/Forums/ope...tml#post370405 http://www.cfd-online.com/Forums/ope...tml#post366429 They seem to have quite basic setup...
__________________
Daniele Vicario blueCFD2.1 - Windows 7 |
|
January 8, 2013, 04:28 |
|
#6 |
Member
Simone
Join Date: Sep 2012
Posts: 95
Rep Power: 14 |
Thank you for the answer Daniele but I had already tried and it didn't work..
|
|
January 9, 2013, 11:13 |
|
#7 | |
Member
Roland
Join Date: Mar 2009
Location: Netherlands
Posts: 92
Rep Power: 17 |
As far as I know you can't get more stable/diffusive than with the settings printed below.
Possibly you can add some (cell/face) limiter on your gradient scheme (see for example http://www.openfoam.org/docs/user/fv...hp#x20-1120118 or http://openfoamwiki.net/index.php/Op...guide/Limiters or http://www.cfd-online.com/Forums/ope...tml#post281280). Is it possible for you to share your setup? Regards, Sylvester Quote:
|
||
January 9, 2013, 12:12 |
|
#8 | |
Member
Simone
Join Date: Sep 2012
Posts: 95
Rep Power: 14 |
Sure sylvester!
Quote:
cheers Simone |
||
January 9, 2013, 12:38 |
|
#9 |
Member
Roland
Join Date: Mar 2009
Location: Netherlands
Posts: 92
Rep Power: 17 |
Hi,
Did you start the adjoint calculation with a (roughly) converged primal result? In my experience this is often required. Also updating the 'alpha' field only after you obtain a (roughly) converged adjoint field helps as well. Did you use a custom boundary condition/cost function, or did you use the one supplied with adjointShapeOptimizationFoam? Are you sure your mesh quality is as good as you can get it? The transition from the prism layers to the rest of the domain appears to be a bit coarse to me. regards, Sylvester |
|
January 9, 2013, 12:54 |
|
#10 |
Member
Simone
Join Date: Sep 2012
Posts: 95
Rep Power: 14 |
Dear sylvester,
I'm performing shape optimization, not topological optimization as performed by adjointShapeOptimizationFoam solver, so I don't have the alpha field. Instead, I can confirm you that the primal field that I use is "at convergence", so I don't think the problem is that. By the way I suspect, as you said, that the problem could be with the transition between the "boundary layer" and the outer cells..so it could be a good idea to refine that zone? With the primal field no problem appears, but I think that the adjoint problem is a "bit" more sensitive.. |
|
January 11, 2013, 11:16 |
|
#11 |
Member
Roland
Join Date: Mar 2009
Location: Netherlands
Posts: 92
Rep Power: 17 |
Hi Simone,
I'm afraid I can't help you further, as it appears you have already tried all the easy solutions. I am curious though if improving your mesh solved the problem. regards, Sylvester |
|
January 15, 2013, 03:58 |
|
#12 |
Member
Simone
Join Date: Sep 2012
Posts: 95
Rep Power: 14 |
Hi again sylvester..I wanted to tell you that the divergence starting from the "spot" has disappeared. Actually, it turned out that checkMesh was failing with the non-orthogonality error..once I've corrected it, that divergence didn't showed up again. However I'm facing another trouble, now at the farfield. Have you ever experienced with your simulations a kind of instability that raises from there? I've tried to change the boundary conditions for the adjoint problem passing from "fixedValue" to "zeroGradient" both for adjoint velocity and adjoint pressure, but the error still remains..any idea??
P.s. now the checkMesh doesn't report any error Cheers Simone |
|
January 15, 2013, 04:33 |
|
#13 |
Member
Roland
Join Date: Mar 2009
Location: Netherlands
Posts: 92
Rep Power: 17 |
Hi Simone,
Is it possible for you to share (pictures of) your case? It would really help in diagnosing possible problems. Regarding the instability you see, does it resemble the one shown in the second picture in this post? http://www.cfd-online.com/Forums/ope...tml#post366429 regards, Sylvester |
|
January 15, 2013, 06:32 |
|
#14 |
Member
Simone
Join Date: Sep 2012
Posts: 95
Rep Power: 14 |
I'll upload them as soon as possible! by the way it seems that the divergence occurs at the farfield to you too..did you fix the problem in some way?
|
|
January 15, 2013, 09:13 |
|
#15 |
Member
Simone
Join Date: Sep 2012
Posts: 95
Rep Power: 14 |
Here's the images sylvester..what do you think? Although the simulation has already "diverged" (take a look to the magnitudes) the problem starts from there..in that edge inlet and outlet patch touch..
let me know what do you think about it cheers Simone |
|
January 15, 2013, 12:31 |
|
#16 |
Member
Roland
Join Date: Mar 2009
Location: Netherlands
Posts: 92
Rep Power: 17 |
Hi,
Unfortunately the only conclusion I can draw from those pictures is: yes, your solution has diverged. For me to even start trying to help, I really need more information than that. Regarding the problem in the other thread. The solution strategy I gave in the second post of that thread (i.e. pseudo staggered approach) did help a lot. Unfortunately I cannot provide you with the resulting code. regards, Sylvester |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Problem with torque output from a turbine simulation. | pa-dundas | FLUENT | 5 | July 17, 2022 06:27 |
Domain format problem on airfoil flow simulation | andrenonaka | CFX | 14 | December 7, 2015 01:42 |
Transient simulation (Problem with massflow and Pressure) | ChristianF | CFX | 4 | August 22, 2011 22:42 |
about valve closing problem during ANSYS FSI simulation | ivy | CFX | 4 | June 8, 2011 22:01 |
Heat Transfer simulation: No convergence problem | fiqs | CFX | 2 | April 21, 2010 16:47 |