Regd. bigParticle voidfraction model

Submitted by Somnath on Tue, 11/13/2012 - 03:34

Hi,

I read in the documentation for the bigParticle voidfraction model that:

The bigParticle voidFraction model is supposed to be used when a particle (or it's representation) is bigger than a CFD cell. The voidfraction field is set in those cell whose centres are inside the particle which results in a stairstep representation of the bodies within the mesh (i.e. voidfraction is either 1 (fluid) of zero (solid)). For archiving accurate results, approx. 8 cells per particle diameter are necessary.

The region of influence of a particle can be increased artificially by "scaleUpVol", which blows up the particles, but keeps their volume (for voidfraction calculation) constant.

Does this mean that the voidfraction will be set to zero, if the center of a CFD cell lies inside the particle when the scaleUpVol is 1.0 ? If that is so, where do we use the alphaMin value (since the minimum voidfraction now will be 0) ?

So far I have seen (without concerning about the accuracy of results) that when I have approximately 2 cells per particle diameter and scaleUpVol of 20, the code runs till the end. But if I try to increase it to 10 cells per particle dia (as suggested in the documentation) and make the scaleUpVol = 1, the code crashes as soon particles are enter the CFD domain.

If someone who has a better understanding of the model, please explain what the documentation means or have any suggestions/insights, then it will be much appreciated.

Thanks
Som

Forums:

Somnath | Tue, 12/04/2012 - 17:01

Hello all,

It's good to have the site back up again :)

If anyone could throw some light on the bigParticle model, I would be very grateful.

Regards
Som

alice's picture

alice | Wed, 12/05/2012 - 14:33

Hi Som,
when running IB cases I would suggest using the voidfraction model "IB", as done in the tutorial case.
Cheers,
Alice

rqwang | Wed, 12/05/2012 - 17:42

Hi Som,

From my experience (I contributed the Gaussian void fraction), gaussian method distribute the void fraction inside and around the particle. Therefore, you may not see total hollow cells in that model. For others, I am not sure. Thx.

rq

Somnath | Wed, 12/05/2012 - 20:14

Hi Alice,

Thanks for your reply! I have a question, is the bigParticle model for unresolved CFD-DEM where the particle dia is bigger than the CFD cell? I am actually trying to run cases where the particle diameter is close to the size of the CFD cell (ideally CFD cell/dia = ~ 0.5) and I am using the bigParticle model because the other models (divided and Gaussian) were crashing.

I have also tried to take a finer CFD grid and use the void fraction IB model, but the simulation blows up very soon and I am still trying . Any suggestions/comments will be very helpful.

Hi rq,

Thanks for your suggestion. I have been trying to work with the Gaussian void fraction model but my simulation crashes with it every time. Under what conditions should it be used you think? As I mentioned above, my CFD cell/particle dia = ~0.5 and particle conc. <=0.3. Any comments will be very helpful.

Cheers
Som

cgoniva's picture

cgoniva | Thu, 12/06/2012 - 13:18

Hi Som,

generally spoken, the particles should be smaller than the cells (cell/particle diameter= ~3). Everything else will lead to errors especially for dense packings. So bigParticle model for unresolved CFDEM is just a quick fix and cannot be recommended!

You either have to use coarser cells - or switch to resolved CFDEM.

Cheers,
Chris

Jing Lu | Mon, 06/02/2014 - 16:04

Hi Chris,

I have been using unresolved CFDEM for a while and recently thinking about using multi particle size. But I don't want to sacrifice much of the fluid mesh resolution in my case.

I understand that bigParticle model is to help decrease the fluid-particle size ratio (down to ~1.0 according to Link et al. 2005), while in resolved CFDEM the fluid-particle size ratio is suggested as 0.1 (Kloss et al. 2012). Correct me if i am wrong about this.

What if I need particles both larger and smaller than the surrounding fluid cells? Do we have a possible compromised solution?

Thanks in advance for your help,
Jing

Somnath | Thu, 12/06/2012 - 20:53

Chris,

Thanks for your comments! I have a few quick (and stupid :) question regarding the resolved CFDEM.

1. I was looking at the twoSphereGlowinski tutorial, and I noticed that, CFD/0/ doesn't have rho although both ShirgaonkarIB and ArchimedesIB require rho. Is rho just assumed to be 1 for these calculations and/or if I specify rho will it matter?

2. I know that the pressure in CFD/0/p is actually p/rho, so is the solution rho independent? Therefore, if I use patchAverage or probes to calculate p at inlet/outlet for pressuredrop, do I need to multiply by rho to get the real pressure drop in Pa?

3. In the resolved CFDEM, does the ShirgaonkarIB takes care of the momentum exchange between DEM and CFD (no momcouple is required in couplingproperties)?

Thanks again!

Cheers
Som

cgoniva's picture

cgoniva | Wed, 12/12/2012 - 00:33

Hi Som,

1.) yes, we assume rho to be 1, see crestFields.H of the IB solver
2.) as in OpenFOAM's incompressible solvers p/rho is used - so your result will also be p/rho. so choose µ,nue and rho (nu=µ/rho) accordingly to get your desired flow.
3.)as seen in the tutorial cases couplingProperties file, no extra momCoupleModel is needed as the solver inherently handles this coupling by fictitiousDomainMethod.

Cheers,
Chris