CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Boundedness of alpha1 in twoLiquidMixingFoam and interMixingFoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 4, 2012, 11:04
Default Boundedness of alpha1 in twoLiquidMixingFoam and interMixingFoam
  #1
New Member
 
Vinay Ramohalli Gopala
Join Date: Mar 2009
Location: Netherlands
Posts: 13
Rep Power: 8
gopala is on a distinguished road
Hello all,

I tried using twoLiquidMixingFoam and interMixingFoam for simple 3d cases with inlet and outlet boundaries and I notice that the volume fraction (alpha1 and alpha2) becomes unbounded. I have the courant number as low as 0.25. The sample output from such a case:

%------------------------------------------------------------------
diagonal: Solving for alpha1, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver: Solving for alpha2, Initial residual = 0.00256416, Final residual = 1.96744e-17, No Iterations 100
Air phase volume fraction = 0.505585 Min(alpha1) = -0.0177925 Max(alpha1) = 1
Liquid phase volume fraction = 0.00634079 Min(alpha2) = 0 Max(alpha2) = 1
diagonal: Solving for alpha1, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver: Solving for alpha2, Initial residual = 0.00253923, Final residual = 3.84262e-17, No Iterations 100
Air phase volume fraction = 0.505553 Min(alpha1) = -0.0174753 Max(alpha1) = 1
Liquid phase volume fraction = 0.00640491 Min(alpha2) = 0 Max(alpha2) = 1
%------------------------------------------------------------------

I am wondering if someone has similar experience with these solvers?
I would really appreciate suggestions to improve the boundedness of the volume fraction.

Thanks in advance,

Vinay
gopala is offline   Reply With Quote

Old   October 9, 2012, 12:45
Default
  #2
Senior Member
 
Kevin Smith
Join Date: Mar 2009
Posts: 103
Rep Power: 8
kev4573 is on a distinguished road
Vinay,

It looks like the max number of iterations is reached (100), which may indicate the solution never converged for your phase fields. You could try a different interface compression scheme to possibly improve stability. Another possibility is to try tweaking your phase related options in fvSolution.

It might also help to have your test case so other people can reproduce your results.

Kevin
kev4573 is offline   Reply With Quote

Old   October 9, 2012, 13:13
Default
  #3
New Member
 
Vinay Ramohalli Gopala
Join Date: Mar 2009
Location: Netherlands
Posts: 13
Rep Power: 8
gopala is on a distinguished road
Thanks for the reply Kevin. In the case I have shown, I had used a very small tolerance to see if this helps, therefore the maximum number of iterations. I will try to post the case file as soon as possible.
Right now i am trying the same case with a finer mesh and it seems to be going in the right direction.

What do you mean by tweaking phase related options in fvSolution?

Best regards,


Vinay
gopala is offline   Reply With Quote

Old   October 9, 2012, 14:35
Default
  #4
Senior Member
 
Kevin Smith
Join Date: Mar 2009
Posts: 103
Rep Power: 8
kev4573 is on a distinguished road
In my experience, the default linear system solver options are usually sufficient. In fvSolution there is a section for PIMPLE solver settings (see below), the phase specific settings are in bold. The other settings affect general solver stability (velocity, pressure coupling). I'd probably start by increasing the number of alpha correctors and sub cycles.

Code:
PIMPLE
{
    momentumPredictor no;
    nCorrectors     3;
    nNonOrthogonalCorrectors 0;
    nAlphaCorr      1;
    nAlphaSubCycles 2;
    cAlpha          1;
}
kev4573 is offline   Reply With Quote

Old   October 25, 2012, 06:57
Default
  #5
Senior Member
 
Albrecht vBoetticher
Join Date: Aug 2010
Location: Zürich, Swizerland
Posts: 185
Rep Power: 7
vonboett is on a distinguished road
Quote:
Originally Posted by gopala View Post
Hello all,

I tried using twoLiquidMixingFoam and interMixingFoam for simple 3d cases with inlet and outlet boundaries and I notice that the volume fraction (alpha1 and alpha2) becomes unbounded. I have the courant number as low as 0.25. The sample output from such a case:

%------------------------------------------------------------------
diagonal: Solving for alpha1, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver: Solving for alpha2, Initial residual = 0.00256416, Final residual = 1.96744e-17, No Iterations 100
Air phase volume fraction = 0.505585 Min(alpha1) = -0.0177925 Max(alpha1) = 1
Liquid phase volume fraction = 0.00634079 Min(alpha2) = 0 Max(alpha2) = 1
diagonal: Solving for alpha1, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver: Solving for alpha2, Initial residual = 0.00253923, Final residual = 3.84262e-17, No Iterations 100
Air phase volume fraction = 0.505553 Min(alpha1) = -0.0174753 Max(alpha1) = 1
Liquid phase volume fraction = 0.00640491 Min(alpha2) = 0 Max(alpha2) = 1
%------------------------------------------------------------------

I am wondering if someone has similar experience with these solvers?
I would really appreciate suggestions to improve the boundedness of the volume fraction.

Thanks in advance,

Vinay
I had this problem with interMixingFoam once because in the initial field I had some cells where the volume fraction of the first (immiscible?) phase together with the second phase added up to a higher value than 1. ( I set the values of phase 2 and 3 to 0.9 and 0.1 with setFields in that region and forgot to set phase 1 to 0 there)
vonboett is offline   Reply With Quote

Reply

Tags
alpha1, boundedness, intermixingfoam, twoliqiuidmixingfoam

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



All times are GMT -4. The time now is 23:32.