
[Sponsors] 
Behaviour of the kOmegaSST in a steadystate case 

LinkBack  Thread Tools  Search this Thread  Display Modes 
June 23, 2015, 07:53 
Behaviour of the kOmegaSST in a steadystate case

#1 
New Member
Max T
Join Date: Feb 2015
Posts: 8
Rep Power: 6 
Hi everybody,
I have a problem with the convergence behavior of my simulation. It is a external and internal aerodynamic simulation of a reference car in a wind tunnel. It is steady state and uses the kOmegaSST turbulence model. The radiator is modelled by a porous media using the fvOptions. The rotating wheels are simulated by a rotating wall BC a the rotationally symmetric parts of the wheel (so mainly the tire) and a MRF Region for each wheel (mainly the rims). The movement of the floor is built like in a wind tunnel using a five belt system (so only moving wall BC). The final flow speed is 60m/s. I say "final flow Speed" because I started to simulate it with a speed of 5m/s. In this case all values except Omega startet so converge immediately. Omega's Initial redidual stayed constant for the first 400 timesteps and I reached my convergence criteria after 1900 timesteps. Now I startet a simulation with 20m/s and Omega shows the nearly the same behaviour with the small difference, that it still (after 1600 timesteps) didn't start to converge. And now I am worrying about the 60m/s simulation, because I haven't enough time to wait for thousands of timesteps untill it starts to converge. I think it is a numerical problem of the Omega solver. I am using a smoothSolver and I think it stucks at a local Optimum of the solution. I forgot to say, that i use the solver simpleFoam. Of course you need at least the fvSolution and the fvSchemes to help me and I will upload it at this evening. About the geometry I can only say, that it is a pretty complex geometry with at about 10 Million cells. Do you need some other files than the both fvS... files? Thank you very much for your help. Max 

June 23, 2015, 08:53 

#2 
Member
Jan
Join Date: Jul 2009
Location: Hamburg
Posts: 72
Rep Power: 15 
Hi Max,
output of checkMesh would also be helpfull. 

June 23, 2015, 14:25 

#3  
New Member
Max T
Join Date: Feb 2015
Posts: 8
Rep Power: 6 
Hi,
here are the files. Firstly the output of checkMesh Quote:
Quote:
Quote:
Max 

June 24, 2015, 03:42 

#4 
New Member
Max T
Join Date: Feb 2015
Posts: 8
Rep Power: 6 
Hi,
additionally I started a transient case this morning using the pimpleFoam solver and kEpsilon. Maybe the local turbulence is too high to solve this case as global steadystate. Max 

June 25, 2015, 09:51 

#5 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 22 
Hey Max, as I understand your first post, it is the outer (SIMPLE) iterations that don't converge for omega. Then, you write about the omega solver itself, but this is related to the inner / linear iterations. Why do you expect an error in the inner solver, when the outer iterations are stuck?
__________________
The skeleton ran out of shampoo in the shower. 

June 25, 2015, 10:04 

#6 
Member
Jan
Join Date: Jul 2009
Location: Hamburg
Posts: 72
Rep Power: 15 
Hi Max,
some ideas: the more complex the flow (mesh) the more iterations you need to have a converged solution. More than e.g. 2000 is quite normal in my experience. LimitedLinear for turbulence equations is optimistic, try linearUpwind (see motorBike tutorial) or even upwind, of course only for the turbulence equations. Also try limited schemes for laplacian and snGrad schemes, e.g 0.5 Best regards, Jan 

June 29, 2015, 08:02 

#7 
New Member
Max T
Join Date: Feb 2015
Posts: 8
Rep Power: 6 
Hi,
Thanks for the good ideas. I startet a simulation using the recommended changes at the fvSolution last Friday. I also changed the speed to an inlet velocity of 60m/s. But the simulation stopped after 6 timesteps. I will upload the logfile this evening. Max 

June 29, 2015, 08:55 

#8 
Super Moderator

Hello Max,
1900 Iterations are not really a lot of iteration. In my combustion solver I have to run something like 30.000 Iterations till I reach a steady state situation. This always depend on the initial values of your simulation. You can use the previous lower velocity solution and start with that but with a higher velocity inlet. That helps a lot in convergence and speed up the simulation. Thus, you can use renumberMesh to speed up your case too. What about your relaxation of omega? I hope you did not forget to set this because in the standard tutorials there is no omega included (as far as I know). If your problem is complex, maybe the mesh should be improved, or your BC are not really a good choice. Relaxation is a topic too and of course all the stuff what is mentioned above. Good luck.
__________________
Keep foaming, Tobias Holzmann 

June 29, 2015, 09:42 

#9 
New Member
Max T
Join Date: Feb 2015
Posts: 8
Rep Power: 6 
Hi Tobi,
I have set a relaxation for omega from the start. As rodriguezFatz said, it's a problem with the simple algorithm. Using pimplefoam there is no problem at all, but I'd really like to use simplefoam. My BC I checked several times, but there could be a mesh problem. Seading my case with a one with a lower velocity I was also thinking about, maybe that's the best I could do. Except from waiting... I will try your ideas this evening. Maybe I'm wrong, but can't I also use the slower simple case for a fast pimple case? Thank you very much. Max 

June 29, 2015, 09:44 

#10 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 22 
You need to post the log file for better assistance.
Edit: I am not quite sure if you understood what I meant in my post.
__________________
The skeleton ran out of shampoo in the shower. 

June 30, 2015, 03:45 

#11 
Senior Member
Francesco Del Citto
Join Date: Mar 2009
Location: Zürich Area, Switzerland
Posts: 233
Rep Power: 13 
Hi Max,
Your mesh is not great, but you should be able to obtain a solution. What are your initial condition? Have you tried to initialise the flow with potentialFoam? This usually helps a lot. Cheers, Francesco 

July 2, 2015, 02:49 

#12  
New Member
Max T
Join Date: Feb 2015
Posts: 8
Rep Power: 6 
Hi,
I think the main BC's should be correct. Inlet U fixedValue (60,0,0) p zeroGradient omega fixedValue k zeroGradient nut calculated Outlet U zeroGradient p fixedValue 0 omega inletOutlet k zeroGradient nut calculated Walls U fixedValue (0,0,0) p zeroGradient omega omegaWallFunction $internalField k kqRWallFunction $internalField nut nutkWallFunction $internalField 5beltsystem U movingWallVelocity (60,0,0) p zeroGradient omega omegaWallFunction $internalField k kqRWallFunction $internalField nut nutkWallFunction $internalField car U fixedValue (0,0,0) p zeroGradient omega omegaWallFunction $internalField k kqRWallFunction $internalField nut nutkWallFunction $internalField car_tires U rotatingWallVelocity p zeroGradient omega omegaWallFunction $internalField k kqRWallFunction $internalField nut nutkWallFunction $internalField Direction and rotational speed is checked car_rims Here I created cellZones with topoSet and defined MRFZones with the fvOptions. Same values and axes as the tires. So I think the BCs of the Inlet and the outlet could be improved, but I thought, that it should be already runable with these BCs. I was using potentialFoam every case I was running, but this time I tried the argument initialiseUBCs. But the simulation stopped after 10 timesteps. Here the logfile: Quote:
Max 

July 2, 2015, 03:04 

#13 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 22 
Well I would run it with
Code:
laplacianSchemes { default Gauss linear uncorrected; } divSchemes { default bounded Gauss upwind; div((nuEff*dev(T(grad(U))))) Gauss linear; }
__________________
The skeleton ran out of shampoo in the shower. 

July 2, 2015, 07:24 

#14 
New Member
Max T
Join Date: Feb 2015
Posts: 8
Rep Power: 6 
Hi,
with these ones it runs, thanks a lot! Done 22 timesteps till yet, because my regular computer isn't available. See residuals, I think convergence behaviour is ok. Thanks a lot, I will post again as the run has completed. Max 

July 2, 2015, 07:30 

#15 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 22 
You can usually get rid of these "bounding Omega" errors by switching off the laplacian correction (> "Gauss linear uncorrected"). You could also do that just for the omega laplacian.
Also of course divScheme upwind is much more stable than your previous scheme.
__________________
The skeleton ran out of shampoo in the shower. 

July 2, 2015, 07:38 

#16  
Super Moderator

Quote:
Maybe you can switch to a high order scheme after a few timesteps, or even after the solution is converged to improve your gradients.
__________________
Keep foaming, Tobias Holzmann 

October 30, 2018, 14:10 

#17  
Member
Join Date: Jul 2015
Location: Gainesville,FL
Posts: 93
Rep Power: 6 
Quote:
Thanks, Rdf 

October 31, 2018, 09:03 

#19  
Member
Join Date: Jul 2015
Location: Gainesville,FL
Posts: 93
Rep Power: 6 
Quote:
I just want to share some experience. And I think the steadystate solution for high numerical Reynolds number simulation (rhoVL/(miu+miu_t)) with RANS, the numerical solution itself may be just a tradeoff between order accuracy (diffusion and dispersion error, etc) and absolute convergence (stability and residual). There is no wellgrounded practice guidance. The actual usefulness of the solution is religious. Someone please correct me if I understand this problem wrong (I think I am absolutely wrong on this, but I can not interpret my experience in another possible way...). "1900 Iterations are not really a lot of iteration. In my combustion solver I have to run something like 30.000 Iterations till I reach a steady state situation." Can you share some details of your simulation? the complexity of your geometry, M, Re, model,etc. And also how satisfied you are with your steadystate solution? Thanks, Rdf 

Tags 
convergence problem, k omega sst, simplefoam 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
plz help,urgent, vof model steady state  Garima Chaudhary  FLUENT  4  March 15, 2018 13:22 
is it possible to predict how long it takes to reach steady state solution in unstead  Alimohamadi_nasr  CFX  4  November 11, 2013 07:11 
steady state, laminar vof_model  Garima Chaudhary  FLUENT  0  May 24, 2007 04:11 
Damp turbulent behaviour for a steady state calculation  andimb  OpenFOAM Running, Solving & CFD  0  May 4, 2006 06:39 
About the difference between steady and unsteady problems  Lisa  Main CFD Forum  11  July 5, 2000 15:37 