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

Alpha1 is reducing.....

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

Like Tree1Likes
  • 1 Post By akidess

Reply
 
LinkBack Thread Tools Display Modes
Old   October 16, 2012, 05:10
Unhappy Alpha1 is reducing.....
  #1
Member
 
Stefano
Join Date: Jul 2009
Posts: 34
Rep Power: 7
Whyman is on a distinguished road
Hi guys,

i have a problem with alpha1 in openFoam 1.6 ext. The value reduces with the time. Here is the output:



/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM Extend Project: Open source CFD |
| \\ / O peration | Version: 1.6-ext |
| \\ / A nd | Web: www.extend-project.de |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 1.6-ext
Exec : interGravitationalFoam
Date : Oct 16 2012
Time : 10:56:34
Host : Alderaan
PID : 3367
Case : /media/F2D48837D487FFD9/LAVORO/OPENFOAM/REXUS/test
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0


Reading g

Loading Accelerations.data

Loading Omega.data
Calculating field g.h


Reading inertial Origin

Reading field pd

Reading field alpha1

Reading field U

Reading/calculating face flux field phi

Reading transportProperties

Selecting incompressible transport model Newtonian
Selecting incompressible transport model Newtonian
Selecting turbulence model type RASModel
Selecting RAS turbulence model kOmegaSST
kOmegaSSTCoeffs
{
alphaK1 0.85034;
alphaK2 1;
alphaOmega1 0.5;
alphaOmega2 0.85616;
gamma1 0.5532;
gamma2 0.4403;
beta1 0.075;
beta2 0.0828;
betaStar 0.09;
a1 0.31;
c1 10;
}

time step continuity errors : sum local = 0, global = 0, cumulative = 0
DICPCG: Solving for pcorr, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 0, global = 0, cumulative = 0
Courant Number mean: 0 max: 0 velocity magnitude: 0
Omega1 initialized to (0 0 0)
Omega2 initialized to (0 0 0)

Starting time loop

Courant Number mean: 0 max: 0 velocity magnitude: 0
deltaT = 0.000595238
Time = 0.000595238

Calculating field g.h

Setting accelerations to (-112.644 1.09078 -0.109779)
Setting omega to (-0.00875158 -0.0815817 0.0820055)
Time at instant 1 is: 0
Time at instant 2 is: 0.000595238
Omega at instant 1 is: (0 0 0)
Omega at instant 2 is: (-0.00875158 -0.0815817 0.0820055)
Instantaneous angular acceleration is: (-14.7027 -137.057 137.769)
Previous Liquid phase volume fraction = 2.25683e-07 Min(alpha1) = 0 Max(alpha1) = 1
DILUPBiCG: Solving for alpha1: solution singularity
Liquid phase volume fraction = 2.25683e-07 Min(alpha1) = 0 Max(alpha1) = 1
DICPCG: Solving for pd, Initial residual = 1, Final residual = 9.62755e-08, No Iterations 329
time step continuity errors : sum local = 1.16224e-11, global = -1.58311e-23, cumulative = -1.58311e-23
time step continuity errors : sum local = 1.16224e-11, global = -1.58311e-23, cumulative = -3.16623e-23
DILUPBiCG: Solving for omega, Initial residual = 0.000655187, Final residual = 1.02048e-07, No Iterations 1
DILUPBiCG: Solving for k, Initial residual = 1, Final residual = 1.13822e-06, No Iterations 1
ExecutionTime = 27.63 s ClockTime = 27 s

Centre of Mass: (3.14552e-07 -4.44441e-05 0.000106692)

Courant Number mean: 0.000712776 max: 0.0760438 velocity magnitude: 10.4599
deltaT = 0.000705782
Time = 0.00130102

Calculating field g.h

Setting accelerations to (-113.489 1.10463 -0.123626)
Setting omega to (-0.00919504 -0.0653216 0.0650064)
Time at instant 1 is: 0.000595238
Time at instant 2 is: 0.00130102
Omega at instant 1 is: (-0.00875158 -0.0815817 0.0820055)
Omega at instant 2 is: (-0.00919504 -0.0653216 0.0650064)
Instantaneous angular acceleration is: (-0.628319 23.0383 -24.0855)
Previous Liquid phase volume fraction = 2.25683e-07 Min(alpha1) = 0 Max(alpha1) = 1
DILUPBiCG: Solving for alpha1, Initial residual = 0.00503263, Final residual = 5.05418e-09, No Iterations 2
Liquid phase volume fraction = 2.25683e-07 Min(alpha1) = 0 Max(alpha1) = 0.892477
DICPCG: Solving for pd, Initial residual = 0.918833, Final residual = 9.18764e-08, No Iterations 329
time step continuity errors : sum local = 1.97884e-11, global = 3.14334e-22, cumulative = 2.82672e-22
time step continuity errors : sum local = 1.97884e-11, global = 3.14334e-22, cumulative = 5.97006e-22
DILUPBiCG: Solving for omega, Initial residual = 0.000743617, Final residual = 2.82979e-08, No Iterations 1
DILUPBiCG: Solving for k, Initial residual = 0.333835, Final residual = 2.95525e-07, No Iterations 1
ExecutionTime = 46.73 s ClockTime = 47 s

Centre of Mass: (1.9406e-07 -3.56954e-05 8.55697e-05)

Courant Number mean: 0.000676682 max: 0.0735919 velocity magnitude: 8.53713
deltaT = 0.000839638
Time = 0.00214066

Calculating field g.h

Setting accelerations to (-114.494 1.1211 -0.1401)
Setting omega to (-0.0097226 -0.0459778 0.0447833)
Time at instant 1 is: 0.00130102
Time at instant 2 is: 0.00214066
Omega at instant 1 is: (-0.00919504 -0.0653216 0.0650064)
Omega at instant 2 is: (-0.0097226 -0.0459778 0.0447833)
Instantaneous angular acceleration is: (-0.628319 23.0383 -24.0855)
Previous Liquid phase volume fraction = 2.25683e-07 Min(alpha1) = 0 Max(alpha1) = 0.892477
DILUPBiCG: Solving for alpha1, Initial residual = 0.00309017, Final residual = 2.7438e-06, No Iterations 1
Liquid phase volume fraction = 2.25688e-07 Min(alpha1) = -1.11844e-97 Max(alpha1) = 0.824762
DICPCG: Solving for pd, Initial residual = 0.617329, Final residual = 9.87751e-08, No Iterations 287
time step continuity errors : sum local = 1.2306e-11, global = -1.7362e-24, cumulative = 5.95269e-22
time step continuity errors : sum local = 1.2306e-11, global = -1.7362e-24, cumulative = 5.93533e-22
DILUPBiCG: Solving for omega, Initial residual = 0.000872859, Final residual = 9.36405e-09, No Iterations 1
DILUPBiCG: Solving for k, Initial residual = 0.263603, Final residual = 1.13085e-07, No Iterations 1
ExecutionTime = 64.18 s ClockTime = 64 s

Centre of Mass: (1.11854e-07 -3.07893e-05 7.3643e-05)

Courant Number mean: 0.00056678 max: 0.0512143 velocity magnitude: 5.03397
deltaT = 0.00099707
Time = 0.00313773

Calculating field g.h

Setting accelerations to (-115.687 1.14066 -0.159662)
Setting omega to (-0.0103491 -0.0230069 0.0207683)
Time at instant 1 is: 0.00214066
Time at instant 2 is: 0.00313773
Omega at instant 1 is: (-0.0097226 -0.0459778 0.0447833)
Omega at instant 2 is: (-0.0103491 -0.0230069 0.0207683)
Instantaneous angular acceleration is: (-0.628319 23.0383 -24.0855)
Previous Liquid phase volume fraction = 2.25688e-07 Min(alpha1) = -1.11844e-97 Max(alpha1) = 0.824762
DILUPBiCG: Solving for alpha1, Initial residual = 0.00133358, Final residual = 3.93363e-07, No Iterations 1
Liquid phase volume fraction = 2.25688e-07 Min(alpha1) = -5.272e-08 Max(alpha1) = 0.79509



I have set buoyantPressure for p and pd and I run a modified interFoam.

Why do I have this result???

Please help me!!!
Whyman is offline   Reply With Quote

Old   October 16, 2012, 05:16
Default
  #2
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 919
Rep Power: 17
akidess will become famous soon enough
You don't give a lot of info, but try using explicit MULES for alpha1. Use a bounded divergence scheme and first order Euler.
__________________
*On twitter @akidTwit
*Spend as much time formulating your questions as you expect people to spend on their answer.
*Help define the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oam-technology
akidess is offline   Reply With Quote

Old   October 16, 2012, 05:36
Default
  #3
Member
 
Stefano
Join Date: Jul 2009
Posts: 34
Rep Power: 7
Whyman is on a distinguished road
Which info do you need in particular?

I set MULES as Explicit, and Euler as time scheme. I don't know exactly what you mean with "bounded scheme"

Anyway it doesn't change, but still gives back the same error.
Whyman is offline   Reply With Quote

Old   October 16, 2012, 05:42
Default
  #4
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 919
Rep Power: 17
akidess will become famous soon enough
Helpful information would be the content of fvSchemes and fvSolution, specifying if you have any special boundary conditions (contact angles, inlets/outlets), or a problematic mesh.

About the bounded schemes - see "4.4.1.1 Schemes for strictly bounded scalar fields" in the user guide. Examples of such schemes are vanLeer01 and Gamma01.

- Anton

Quote:
Originally Posted by Whyman View Post
Which info do you need in particular?

I set MULES as Explicit, and Euler as time scheme. I don't know exactly what you mean with "bounded scheme"

Anyway it doesn't change, but still gives back the same error.
__________________
*On twitter @akidTwit
*Spend as much time formulating your questions as you expect people to spend on their answer.
*Help define the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oam-technology
akidess is offline   Reply With Quote

Old   October 16, 2012, 05:51
Default
  #5
Member
 
Stefano
Join Date: Jul 2009
Posts: 34
Rep Power: 7
Whyman is on a distinguished road
Ok, I attach all the files for boundary condition plus fvSolution and fvScheme.

There is the contact angle acting in the domain.
Attached Files
File Type: zip 0.zip (13.9 KB, 9 views)
File Type: txt fvSchemes.txt (2.3 KB, 14 views)
File Type: txt fvSolution.txt (3.0 KB, 8 views)
Whyman is offline   Reply With Quote

Old   October 16, 2012, 06:50
Default
  #6
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,077
Blog Entries: 4
Rep Power: 19
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Quote:
Originally Posted by Whyman View Post
Ok, I attach all the files for boundary condition plus fvSolution and fvScheme.

There is the contact angle acting in the domain.
Hi Whyman (nice name by the way)



Your Problem description
- - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - -

I can not see any problem in your case. You said that the value of alpha1
goes below 1. Thats does not mean to be an error or an numerical problem. I had a look
in your time folder 0 and saw that there is no inlet for alpha1 that is
set to fixedValue.


I have got a notation that ...
- - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - -
you are init your alpha1 with the setFields command in a certain
region (like the damnBreak tutorial). While solving your case
the fraction 1 is distributed in the region (maybe due to gravitation)
and your fraction value reaches values below 1 due to distribution and the
fact that your fraction 1 is a thin layer or something like that.

Further more: You set your BC for U to fixedValue (0 0 0).
So I expect that you are in a closed box or sth. like that.


Experience
- - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - -
A year ago I made a simulation of a chocolate donot. Therefor I set a chocolate
field like a plate into my mesh and let it fall down on my donut due to gravitation.
I realized that the fraction is distributed due to the gravitation and velocity becouse
my chocolate plate was very thin and I used the visco of water and not of chocolate,
The results was, that my maxAlpha1 value goes down below 1.

That was logical couse the cells which belong to alpha1 = 1 take a high of 4 cells.
After the first few timesteps I got values below 1. I had a look at the first calculation
steps and realized that problem.


To do
- - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - -
First of all, write out the first time steps and have a look at it with paraview.
It should be possible to see your problem, or if your calculation is correct or wrong.

If everything is okay check your boundary conditions, initialization and so on. After
that you can go on and check your schemes. Like akidess told you use first order euler schemes
for time derivation and bounded scheme for alpha1.

But if the problem occure with MULES and DILUPBiCG it seems like the problem I mentioned and that
its not a problem in the numerical schemes.

I have no idea about your geometry and initialization but I think its due to distribution of the fraction
and the value goes under 1 couse your fraction 1 is a thin layer or sth. like that.


Further more
- - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - -
its possible that I skipped some details?.?.?
Without a concrete case I can not help you.
I grope on the dark.


But I Hope that this will help you a bit


Regard
Tobi

Last edited by Tobi; October 16, 2012 at 07:05. Reason: Adding some lines
Tobi is offline   Reply With Quote

Old   October 16, 2012, 07:04
Default
  #7
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 919
Rep Power: 17
akidess will become famous soon enough
I agree with Tobi. I understood your original problem as that the volume integral of alpha1 is reducing (i.e. you are losing mass), but now I realized you meant that your maximum value is reducing (i.e. your field is dispersing). Follow the steps suggested by Tobi.
Tobi likes this.
__________________
*On twitter @akidTwit
*Spend as much time formulating your questions as you expect people to spend on their answer.
*Help define the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oam-technology
akidess is offline   Reply With Quote

Old   October 16, 2012, 08:27
Default
  #8
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,077
Blog Entries: 4
Rep Power: 19
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi Anton,

i think your word "dispersed" is much common then my word used "distribution"

Tobi
Tobi is offline   Reply With Quote

Old   October 16, 2012, 10:08
Default
  #9
Member
 
Stefano
Join Date: Jul 2009
Posts: 34
Rep Power: 7
Whyman is on a distinguished road
Hi guys,

thanks for your help....

Anyway, the domain is a cylindrical container, with inside some liquid and gas, subjected to acceleration varying with time.

Because I have modified a bit the interFoam solver, i send to you my UEqn and pEqn files: maybe i have made some mistakes in writing the code.

pEqn
{
volScalarField rUA = 1.0/UEqn.A();
surfaceScalarField rUAf = fvc::interpolate(rUA);

U = rUA*UEqn.H();

surfaceScalarField phiU
(
"phiU",
(fvc::interpolate(U) & mesh.Sf())
+ fvc::ddtPhiCorr(rUA, rho, U, phi)
);

adjustPhi(phiU, U, pd);

phi = phiU +
(
fvc::interpolate(interface.sigmaK())*fvc::snGrad(a lpha1)
- ghf*fvc::snGrad(rho)
)*rUAf*mesh.magSf();



for(int nonOrth=0; nonOrth<=nNonOrthCorr; nonOrth++)
{
fvScalarMatrix pdEqn
(
fvm::laplacian(rUAf, pd) == fvc::div(phi)
);

pdEqn.setReference(pdRefCell, pdRefValue);

if (corr == nCorr-1 && nonOrth == nNonOrthCorr)
{
pdEqn.solve(mesh.solver(pd.name() + "Final"));
}
else
{
pdEqn.solve(mesh.solver(pd.name()));
}

if (nonOrth == nNonOrthCorr)
{
phi -= pdEqn.flux();
}
}



U += rUA*fvc::reconstruct((phi - phiU)/rUAf);
U.correctBoundaryConditions();

# include "continuityErrs.H"

p = pd + rho*gh;

if (pd.needReference())
{
p += dimensionedScalar
(
"p",
p.dimensions(),
pRefValue - getRefCellValue(p, pdRefCell)
);
}

}


UEqn

surfaceScalarField muEff
(
"muEff",
twoPhaseProperties.muf()
+ fvc::interpolate(rho*turbulence->nut())
);

fvVectorMatrix UEqn
(
fvm::ddt(rho, U)
+ fvm::div(rhoPhi, U)
- fvm::laplacian(muEff, U)
- (fvc::grad(U) & fvc::grad(muEff))
+ Fcentrifugal
+ Feuler
+ Fcoriolis
//- fvc::div(muEff*(fvc::interpolate(dev(fvc::grad(U)) ) & mesh.Sf()))
);

UEqn.relax();

if (momentumPredictor)
{

solve
(
UEqn
==
fvc::reconstruct
(
(
fvc::interpolate(interface.sigmaK())*fvc::snGrad(a lpha1)
- ghf*fvc::snGrad(rho)
- fvc::snGrad(pd)
) * mesh.magSf()
)
);
}




I have also written the following lines in the main code, to take the gravity variation in account:

dimensionedVector acc("Acceleration", dimAcceleration,it(runTime.timeOutputValue()));
g = acc;

Info<< "Calculating field g.h\n" << endl;
volScalarField gh("gh", g & mesh.C());
surfaceScalarField ghf("gh", g & mesh.Cf());



Maybe now my problem is clearer (I hope).
Whyman is offline   Reply With Quote

Reply

Tags
alpha1

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


Similar Threads
Thread Thread Starter Forum Replies Last Post
Formulation in compressibleInterFoam scttmllr OpenFOAM Running, Solving & CFD 52 May 2, 2015 11:42
interFoam VOF is loosing fluid wersoe OpenFOAM Running, Solving & CFD 13 June 26, 2013 08:13
Problem with interFoam; Wave/wiggle alpha1 behavior JonW OpenFOAM 3 February 23, 2013 21:41
Multiple floating objects CKH OpenFOAM 10 September 21, 2011 23:13
Fixing the alpha1 min/max under/overshoots in interFoam.C solver. idrama OpenFOAM 1 January 27, 2010 20:34


All times are GMT -4. The time now is 20:46.