Velocity and Pressure Problem

Dear CFDEMers

Starting from the settlingTestMPI I build up a case with 729 particles with diam 0.001 in a 0.1x0.01x0.01 simulation box. On the left side of the box there is an Inlet with vmean=1 and on the right side an outlet with p=0. For the box and the particles the Re is <1 which implies the flow is laminar. Running liggghts and OpenFOAM separately there are no problems. I checked the timestep in liggghts with fix check/timestep/gran.
When I couple with CFDEM-Solver and choose a "large" timestep I get a solution although the Co-Number is sometimes higher than 0.5. From the visualization in ParaView it is clear that the solution for U and p is crap. To overcome this problem I reduced the timestep for CFD but then the Co-Number increases until infinity. Then I reduced the Coupling interval and the timestep in CFD and DEM but with no success. Also mesh refining does not help.
I believe that the physical setup (BC, IC, RASModel ans so on) is correct. According to that the solution fails due to solver or coupling adjustment.
1) Whats the best way to get accurate results?
2) When is the keyword dilute for the averagingModel no more feasible?
3) What does centreProps mean?
4) Can anybody give informations about the entries in bigParticleProps?
5) If the mesh for CFD is equal or smaller respective to the particle size is that a problem?

Thanking you in anticipation for help.
Cheers
Claudio

Forums:

CFDEM®coupling - User Forum

cgoniva | Mon, 11/14/2011 - 17:45

Hi Claudio! 1) Whats the best

Hi Claudio!

1) Whats the best way to get accurate results?
generally spoken:
-accurate DEM settings
-small coupling interval
-small fluid TS
-fine mesh (see point 5!)
This reduces the truncation errors of discretisation.
2) When is the keyword dilute for the averagingModel no more feasible?
-it is less accurate and only bearable for very dilute regime
3) What does centreProps mean?
-using centre voidFraction calculation means volume of the particle is accounted for only in the cell the centre of the particle is located in. (see point 5!)
4) Can anybody give informations about the entries in bigParticleProps?
-bigParticle void fraction calculation can help you smear out the interaction between particles and fluid - should increase stability, especially if you artificially increase the particle size.
5) If the mesh for CFD is equal or smaller respective to the particle size is that a problem?
-then you run into truble, as a cell is completely covered by a particle - voidfraction reaches 0, equations become crap. (point 4 can help) A good inciator for small mesh size is a very non-uniform voidfraction field and voidfraction < 0.3.

Cheers,
Chris

Claudio Wolfer | Tue, 11/15/2011 - 10:02

centreProps and bigParticleProps entries

Hi Chris

Thanks for answering. That helps a lot. Some more questions arose while studying answers 3) and 4).

centreProps:
a) alpha == voidFraction == fluid volume fraction?
b) alphaMin (in centreProps) specifies the lower bound for voidFraction and makes sure that the equations don't become crap?

bigParticleProps:
c) The maxCellsPerParticle specifies on how many cells around the cell (the center of the particle is located in) the interaction is smeared out? If yes, I have to ensure that the volume of the number of cells is in the same order the particle has?
d) Should the alphaMin be equal to the alphaMin in centreProps? I guess yes, because in the other way I would create a conflict with centreProps.
e) What is scaleUpVol good for?

Bye for now
Claudio

cgoniva | Tue, 11/15/2011 - 12:23

Hi! centreProps: a) alpha ==

Hi!

centreProps:
a) alpha == voidFraction == fluid volume fraction?
yes
b) alphaMin (in centreProps) specifies the lower bound for voidFraction and makes sure that the equations don't become crap?
yes

bigParticleProps:
c) The maxCellsPerParticle specifies on how many cells around the cell (the center of the particle is located in) the interaction is smeared out? If yes, I have to ensure that the volume of the number of cells is in the same order the particle has?
for now the array length of the cells covered by the particle is hard coded to maxCellsPerParticle. In case mor cells are found - an error message will tell you.

d) Should the alphaMin be equal to the alphaMin in centreProps? I guess yes, because in the other way I would create a conflict with centreProps.
This is just a backup to avoid from blowing up - in a perfect world it should not reach that limiter.

e) What is scaleUpVol good for?
artificially increase the particle size to smear out interaction, volume in terms of voidfraction is kept constant to the real particle volume.

Cheers,
Chris

rqwang | Tue, 11/15/2011 - 19:43

Hi Claudio Following Chris, I

Hi Claudio

Following Chris, I would like to add two points:

1) the algorithm for scaleUpVol is
first, derive a new radius Rn=(particle real radius)*pow(scaleUpVol, 0.3333)
Then, the momentum from discrete will be evenly distributed to a sphere with a radius of Rn

2) For my simulation, I always start to use scaleUpVol=200. In that case, the bigParticle model won't affect too much.
With more confidence, I will reduce it to around ~20 and get a reasonable result.

Hope this helps.

Thanks.

Claudio Wolfer | Tue, 11/15/2011 - 14:22

An other pressure problem

The explanations below were very helpful. At the moment my case is solving. I noticed an interesting behavior from the solver when calculating the pressure equations.
In the fvSolution-File I specified nCorrectors to 4. At the beginning I can see the four corrector steps in the solver output. But after each DEM step the solver makes eight corrector steps. The number of corrector steps decreases until the next DEM step to six or four.
Uses the cfdem-Solver a variable number of corrector steps?

I hope my attempt to explain was understandable.
Cheers
Claudio

cgoniva | Wed, 11/16/2011 - 08:34

Hi! >>Uses the cfdem-Solver a

Hi!

>>Uses the cfdem-Solver a variable number of corrector steps?
Yes, it does, see:

// classic PISO control
for (int corr=0; corr