bc's of a komegaSST case
2 Attachment(s)
Hallo,
I have a question concerning the boundary conditions for my special case. I hope I won't bother you, this surely is a quit often stated question, but searching the forum couldn't answer all my questions. The geometry of my case can be seen in the picture below. On the right side of the model is the inlet, on the left side is the outlet. This is just a very simple model of the more complex object, but the effects should appear here as well. And the computation time is much lower, so it is quite good for testing. Right now I am dealing with the boundary conditions and wether to handle the flow as turbulent or laminar. I use the pisoFoam solver and the komegaSST turbulence model. I first used the usual bc (inlet: U value, p zeroGrad; outlet: U zeroGrad, p 0), but I would prefer a pressure value at the inlet and outlet. Because I just get the pressure drop between the two chambers from experiments. Right now I have these bc's: Inlet: U: zeroGradient (better results than inletOultet; almost same results as pressureInletOutletVelocity) p: fixedValue (10.085) k: fixedValue (0.013) omega: fixedValue (8.39) nut: calculated (0) Outlet: U: zeroGradient (better results than inletOutlet; same results as pressureInletOutletVelocity) p: fixedValue (1.51) k: zeroGradient omega: zeroGradient nut: calculated (0) (with inletOutlet at k and omega it does not converge; diverges when the flow reaches the outlet) Walls: U: fixedValue (0 0 0) p: zeroGradient (>noslip) k: kqRWallFunction (0) omega: omegaWallFunction (0) nut: nutWallFunction (0) With these bc's the simulation is converging. My question is, are these boundary conditions ok for my case? I don't like to set these on my personal assumptions. Are there any publications dealing with such boundary conditions where I can rely on? I also did the simulation with a laminar flow, the other parameters remained the same. The results of the laminar case (the second picture) seem more turbulent and chaotic to me. But these effects could occur due to numerical instabilities, what do you think? Another question: When running the case with the komegaSST model the velocity residuals and iterations are not mentioned in the log anymore, why is this? Just not declared to be printed in the code? Maybe anybody has had a similar case and can give me any suggestions or advices. Thanks! 
Nobody?
Why does the turbulence model show so different results than the laminar model? Which one is more appropriate? 
Quote:
i think you are running laminar case with second order scheme and these fuctuations are result of that. RANS model increases effective viscosity so the effect of second order scheme is not visible any more. 
So should I run the case with higher order schemes?

As Arjun said, by using a turbulence model you are increasing the effective viscosity (nu + nut). This means increased dissipation, which will smear out the instabilities in the flow... Using laminar, or a turbulence model depends on what you are trying to simulate  looking at your Reynolds number might help if you have no idea (I don't know what the mean velocity or what type of fluid you want to simulate ).
My gut feeling concerning your b.c. is that you are lucky to get convergence by using zeroGradient conditions both on inlet and outlet. Incorrect initialization might lead to divergence and nonphysical inflows etc... Using pressureInletOutletVelocity b.c. sounds safer in general. 
Thanks you! I have quite high Reynolds numbers, 15002500. And several experimental studies have shown a turbulent behavier of the jet (in the left chamber). So, of course, I first thought about using a turbulent model. But I am not very happy with the results, it doesn't look very physically correct to me. The results of the laminar solver is more what experiments have shown. But I have no good feeling by using it.
Hmm, should I use a very fine mesh, higher order schemes and no model? Just for validation, to compare the results. I am interested in shorter computation time, so this would not be the final approach. What do you think, is the use of a tubulence model the best idea for my case and I just have to accept the results? Ok, you have convinced me, I will use the pressureInletOutletVelocity bc. Should I just use it for the inlet or both the inlet and outlet? Thanks a lot for your help. I don't know who else I could ask. I have read several books about CFD but none could answer these questions. 
What about using LES instead of RANS ? That way you can capture the unsteadiness in your flow ? Refining the mesh in the jet region downstream is definitely essential for accuracy and will also limit the numerical diffusion.
What are your settings in the fvSchemes dict ? 
Yeah, I thought about trying to use LES. I'll do that the next days. Maybe I'll have some questions about the correct parameters to use. I don't know much about LES, yet.
In our more complex model I already have a refined mesh in the area of the orifice and the jet region. I also did some studies how fine the mesh has to be. With the finest mesh I tried, I got the same fluctuations as can be seen above. I'll give you my fvSchemes settings tomorrow when I am back at work. I can't remember all the setting right now. 
So, here are my settings for the fvSchemes dict:
ddtSchemes: Euler I first had Crank Nicholson, but thought this may be too much. Maybe a blending of both is a good option, is it? divSchemes: default Gauss upwind div(phi,U) Gauss linearUpwindV Gauss linear; div(R) Gauss linear; div((nuEff*dev(grad(U).T()))) Gauss linear; The last two setting may be irrelevant for my case. laplacianSchemes: default Gauss linear corrected (nu,U) Gauss linear correced (nuEff,U) Gauss linear limited 0.7 (1A(U)),p) Gauss linear limited 1; (DkEff,k) Gauss linear limited 0.7; (DepsilonEff,epsilon) Gauss linear limited 0.7; (DREff,R) Gauss linear corrected; (DnuTildaEff,nuTilda) Gauss linear limited 0.7; interpolationSchemes; default linear limited 1; snGradSchemes: default corrected And my fvSolution settings: p: GAMG / DICGaussSeidel pFinal: GAMG / GaussSeidel U,k,omega: PBicG /DILU PISO: nCorrectors 2 relaxationFactors: p 0.3; U,k,omega 0.7; So, what are your suggestions? 
I now tried several different settings within the fvSchemes Dictionary. The results are very different when changing the ddtSchemes and the divSchemes. Is this normal or are other parameters wrong (e.g. the BCs)? Can someone please give me any suggestions what settings I should use?
On a very fine mesh I get the best results when I use the backward ddtScheme and the Gauss cubic divScheme (while running icoFoam). But on a coarser mesh there are a lot of instabilities with these settings. I also tried the LES Method. My settings are as follows: ddtScheme: default CrankNicholson 0.6 divScheme: default Gauss upwind div(phi,U) Gauss linearUpwindV Gauss linear div(B) Gauss linear div((nuEff*dev(grad(U).T()))) Gauss linear The other settings are the same as in my previous post. Please help, I really don't know what I should use! Thanks! 
Quote:
(DepsilonEff,epsilon) < shoud have OMEGA (instead of epsilon) I have seen an example that makes use of kOmegaSST and I tried to replicate the files and adjust them to my case. I hope it helps 
Ah, thanks!
I now make use of the LES, not RANS anymore. I use a dynamic SGS (locdynoneeqeddy). This is much better for my lowReynoldsnumber problem, because I have a lot of laminar flow in my domain. RANS dissipates too much energy and there is almost no turbulence anymore (what can be seen in the picture above). But I still don't know wether I should use an upwind scheme (of second order) or CDS for my convective term. Upwind should not be used for LES, because it dissipates too much. But it is very stable and with CDS I get several fluctuations. But I don't know wether these fluctuations are the result of numerical oscillations or actually occur in the flow. I have no opportunity to verify my results with experiments. This makes it quite difficult. Please tell me when you have found a good solution for your (similar) problem. 
All times are GMT 4. The time now is 00:56. 