hello everyone,
I have a question of the implementation of DiFelice drag model in cfd-dem.
the code detail is:
if (magUr > 0)
{
// calc particle Re Nr
Rep = ds*voidfraction*magUr/nuf;
// calc fluid drag Coeff
Cd = sqr(0.63 + 4.8/sqrt(Rep));
// calc model coefficient Xi
scalar Xi = 3.7 - 0.65 * exp(-sqr(1.5-log10(Rep))/2);
// calc particle's drag
drag = 0.125*Cd*rho*M_PI*ds*ds*pow(voidfraction,(1-Xi))*magUr*Ur*voidfraction;
}
when calculating the drag force, why multiply the voidfraction into the drag force ? this seems different with the original version of DiFelice model.
another question: has somebody made a comparison with the experiment of Tsuji(1993,Discrete particle simulation of two-dimensional fluidized bed), the earliest paper describing DEM-CFD coupling?
I take a calculation with the same information as described in the paper. but the particles can't be fluidized.
although many time have been spent on the details of the code, few results have got.
so any hints or suggestions with be very appreciated.
thanks.
S.L
cgoniva | Tue, 09/20/2011 - 16:54
Hi! you will find different
Hi!
you will find different versions of DiFelice in literature. We implemented one which was best suited to other laws like Koch and Hill (which I recommend to use) or Wen and Yu.
We did some tests on fluidized beds and got great results - some publications on that in the pipeline.
But we never did a comparison with the paper you mention.
Cheers,
Chris
skyopener | Wed, 09/21/2011 - 06:51
hi Chris, thanks for your
hi Chris,
thanks for your kindly reply.
I want to take a calculation test with an experiment of Tsuji in order to be familiar with the process of coupling.
After set a case by modifying the HopperFlow tutorials, many problems appear in the calculation.
perhaps some important messages have not been caught in my calculation.
so may i ask you some questions on coupling?
Q#1:
When calculating in parallel, the particles are out of range of fluid domain. the problem lies in the standardsearch model.
it always return cellID=-1 when searching the cell number that particle is in. but the particle's coordinate is in the fluid domain...
so should the domain decomposed with the same number of processors in each direction? for example, if the fluid domain is split as 2*3*2, then LIGGGHTS must be strictly set with 2*3*2? does it matter if we set 4*1*3?
Q#2:
After the appearance of the above problem, I changed the coupling process with TwoWayFile method and run the program serially.
also set the inlet velocity larger than the minimum velocity given in the paper(1.5 times), change the fluid properties to the proper value of air.(the density change from 1 to 1.205 in the 0/rho file, the nu to 1e-05 instead of 1e-4 in the original setting in the CFD/constant/tranportPorperties file)
The fluid domain is calculated using LES.
but the drag force is smaller than the gravity of the particle, and after a long time's debug, few thoughts appear....
any hints will be highly appreciated.
thx!
S.L
cgoniva | Wed, 09/21/2011 - 08:28
Hi SL, when decomposing the
Hi SL,
when decomposing the domain it is obvious that if one proc is trying to locate all particles of the calculation (which is coded currently) it will find only those within his domain - all the others won't be located and won't be further processed by this proc.
Due to above mentioned algorithm (each proc tries to locate every particle) you do not have to choose the same domain size and decomposition in LIGGGHTS and the CFD sim.
Cheers,
Chris
skyopener | Wed, 09/21/2011 - 15:59
Hi Chris, thanks for your
Hi Chris,
thanks for your kindly reply.
with your clear description, more details have been got about the coupling.
and now I'm confidence in the parallel calculation of particle's move.
perhaps my problem lies in the grid size.(The grid is coarse. everyone with 10mm*20mm*8mm in x*y*z direction. and the particle's diameter is 4mm, density = 2700kg/m^3)
so more effort will be taken on a refined grid..except a better result.
thx for your help again...
S.L
ckloss | Wed, 09/21/2011 - 16:03
You can try to use the Koch
You can try to use the Koch and Hill drag model instead of DiFelice - we got better results with this one
Cheers, Christoph
skyopener | Thu, 09/22/2011 - 06:35
hi Christoph, thanks for your
hi Christoph,
thanks for your kindly reply and useful information.
Both drag models have been used in the calculation. and the debug information tells me that the drag force is about 10% of the gravity. so the problem must lie in the value of the fluid velocity' calculation or the volume faction's calculation of the current cell that the particle is in.
more efforts will be paied on information of these values....
many thanks for you.
S.L
cgoniva | Wed, 09/21/2011 - 20:32
Hi! your grid-particle ratio
Hi!
your grid-particle ratio is quite small - at least in z-dir.
If voidfraction field gets too inhomogenious Ksl prediction is erroneous (see Ergun testcase ;-))
you could try to use bigParticle with artificially smeared properties by using scaleUpVolume - this might help...
Cheers,
Chris
skyopener | Thu, 09/22/2011 - 06:54
hello Chris, I sincely
hello Chris,
I sincely appreciate your useful information.
perhaps this information hits the problem in my calculation.
the drag force is calculated using the current cell's velocity and voidfraction,.so it must be the no really velocity value because of the erroneous prediction of Ksl, which leads to a smaller drag force. the drag force is so smaller that the particles can't be fluidized.
thanks for your persist help..
S.L