[tayo]

Hello all,

I'm running rising bubble case using interDyMFoam. The issue is that alpha1 blows up whenever I run with flow velocity i.e. maximum alpha1 grows unbounded beyond 1 and minimum alpha1 also grows beyond zero even after the first time step. However, it behaves fine when I run without flow velocity.

I've tried running implicitly and then played around with the div(phi,alpha) & div(phirb,alpha) in fvSchemes, and then with calpha and nAlphaSubCycles in fvSolution. I've even set maxCo & maxAlphaCo to 0.01 yet it still grows. Please I need ideas on how to make alpha1 stay bounded between 0 and 1 irrespective of flow velocity. I would really appreciate any help. Thank you.

[tayo]

Please I'm still waiting for response/ideas on how to keep alpha1 bounded using interDyMFoam. Thank you.

[Lieven]

Hi Tayo,

A thing you can try (at least this is what I would do) is to select the 'upwind' interpolation for all operators in the fvSchemes. It is first order, so you don't want to keep it, but it is bounded. So you should not get the under/overshoots. Next, replace each upwind by a second order scheme until you see the problem arising. For that operation you need to pick a more advanced scheme (TVD, explicitly bounded scheme, filtered, ...).

Cheers,

Lieven

[tayo]

Thanks Lieven,

I've just tried upward scheme on div(phi,alpha) but it still grows unbounded, then, I tried vanLeer01 but same result. I'm currently using limitedVanLeer 0 1 but it's not looking any different. I'm currently running at time step of 1e-6sec. The wield thing is that when I ran the case without adaptive meshing (interFoam), alpha1 didn't blow up although I had to use maxCo and maxAlphaCo of 0.1. So I strongly think it has to do with interDyMFoam but I don't know how to correct the solver. I really need adaptive meshing for my case.

[Lieven]

hi Tayo,

I really meant to use the upward scheme for all operators as starting point. At this point, there is really no reason yet to think it is a problem of the solver. Low mesh quality or poor initial conditions e.g. are more likely.

Cheers,

L

[tayo]

Update!
I noticed that I got worst void fraction results as I increased calpha and calpha = 0 had "best result" (instead of the reverse occuring). Upward schemes also made it worst as expected too. Could this "unboundedness" be as a result of the interfaceCompression scheme? Any other recommendable schemes for the div(phi, alpha) and div(phirb, alpha)?

[tayo]

Hello all,

I've been able to fix the issue. First of all, I discovered that the problem of unbounded alpha1 was not unique to interDyMFoam alone, it also blew up in interFoam. By the way, my flow velocity was quite high (~1m/s) but alpha1 still blew up even with low vel (~0.01m/s). The div schemes did not help much, neither did a very very low maxAlphaCo (0.01).

To solve it, I solved the solution implicitly setting Sp as zero. But for Su term, I defined as divU*alpha1. This extra divergence term helped keep the alpha1 equation stable along with the right combination of maxAlphaCo. This has kept my max alpha1 bounded to 1 while you won't lose computation time since maxAlphaCo of 0.4 has worked fine. Hope this helps anyone else with unbounded alpha1 issue. Thanks

[k.kshitij]

Hi,

I simulating a nozzle flow using k-e turbulence model in interFoam, and getting a negative phase fraction. I'm a newbie to C programming, can you tell where to add the corrections you have given. I ran a grep command to find out where the SpType is used and found
these locations
applications/solvers/multiphase/interFoam/LTSInterFoam/MULESTemplates.C
src/finiteVolume/fvMatrices/solvers/MULES/MULESTemplates.C

But didnt find where Sp is defined in them, can you please guide me through this.

[tayo]

Originally Posted by k.kshitij

Hi,

I simulating a nozzle flow using k-e turbulence model in interFoam, and getting a negative phase fraction. I'm a newbie to C programming, can you tell where to add the corrections you have given. I ran a grep command to find out where the SpType is used and found
these locations
applications/solvers/multiphase/interFoam/LTSInterFoam/MULESTemplates.C
src/finiteVolume/fvMatrices/solvers/MULES/MULESTemplates.C

But didnt find where Sp is defined in them, can you please guide me through this.

Hi Kshitij, you're probably solving interFoam explicitly. See interPhaseChangeFoam for example on how to add Sp & Su terms and then solve implicitly. You're probably not doing any phase change for now so set Sp to zero. However, to ensure that alpha1 stays bounded, include "divU*alpha1" in the Su term. Hope this helps.

[Hale]

Originally Posted by tayo

Hi Kshitij, you're probably solving interFoam explicitly. See interPhaseChangeFoam for example on how to add Sp & Su terms and then solve implicitly. You're probably not doing any phase change for now so set Sp to zero. However, to ensure that alpha1 stays bounded, include "divU*alpha1" in the Su term. Hope this helps.

Hi Tayo,

I am very new to OpenFoam and C++ coding and I'm facing the same problem as yours where alpha1 becomes negative. Would you please post the files with required changes in order to avoid this problem?

I really appreciate your help.
Hale

[jhoepken]

Originally Posted by Hale

Hi Tayo,

I am very new to OpenFoam and C++ coding and I'm facing the same problem as yours where alpha1 becomes negative. Would you please post the files with required changes in order to avoid this problem?

I really appreciate your help.
Hale

Have you double checked your boundary conditions?

[Hale]

Originally Posted by jhoepken

Have you double checked your boundary conditions?

I solved the problem. There was problems with the boundary conditions :-)

[Galchenko]

Hi Hale!

I'm having the same problem as discussed before, though adding Su term as tayo adviced didn't help. What boundary conditions caused you problem? May be I have some similliar mistake..

Regards,
Olga

[Hale]

Hi Galchenko,

I had zeroGradient on the both pressure and velocity for the inlet and zeroGradient for the velocity and a negative pressure for the outlet, which was equal to the pressure difference between inlet and outlet. This was apparently a very poorly defined boundary condition for my system which made it very unstable and therefore alpha1 became negative.

My intention by setting those boundary conditions was to let the model determine the velocity at the inlet but the system was apparently an overdetermined system which could not be solved in OF.

I changed the BC to the following and it worked fine:

Inlet:
U: fixedValue uniform (x 0 0);
p_rgh: buoyantPressure;

Outlet
U: zeroGradient
p_rgh: fixedValue uniform 0;

[zhouhoucun]

Hello,tayo, I meet the same problem as you with interPhaseChangeFoam, could you send me you case files for me?Thank you in advance

[Nori4U]

Originally Posted by zhouhoucun

Hello,tayo, I meet the same problem as you with interPhaseChangeFoam, could you send me you case files for me?Thank you in advance

Hi Zhouhoucun,

I'm working on the same problem, can you upload your case files please so I can cross check with mine.

Thanks,
Sam