Fluids

Source term convergence issues with a gas-solid model

• Felix_unsw
Subscriber

Hello friends.

I am modeling a transient particle-gas system inside a tube. The particle trajectories are calculated externally using UDFs, so I have to pass back the drag forces as source terms to take into account the effect of the particles on the gas flow.

I found that fluent had difficulty converging in the case of dense particles accumulated in one or more cells (porosity becoming less than 0.5). As a result, the gas flow velocity can suddenly become very high due to the inability to converge.

I tried to reduce the time step of Fluent (gas flow) to 1e-7s, and it worked well for dilute particle cases. But the problem still occurs when more particles are injected. Can anyone give me a suggestion to solve this problem?

Thanks!

*****Here is the udf for source terms*****:

DEFINE_SOURCE(xmom_source,c,t,dS,eqn)

{

real source = 0.;

if(initialized)

{

source = C_UDMI(c,t,1)/C_VOLUME(c,t);

}

dS[eqn] = 0.0;

return source;

}

C_UDMI(c,t,1) stores the drag force on particles.

• Rob
Ansys Employee
I suspect you need to review the amount of drag force that's transmitted when the volume fraction gets high. In a dilute system it's reasonable to assume each particle is separate and adds some momentum to the flow. In a dense system does the drag effect sum, or is it a function of the sum? If you review the Eulerian Granular theory in the manual it may help with the maths and references. As an aside, DPM is valid up to around 12% by volume as particle volume and interaction isn't fully accounted for.
• Felix_unsw
Subscriber
Hi Rob, thank you so much for your reply. My momentum source terms are calculated by summing up the drag force acting on each particle in a fluid cell so that NewtonÔÇÖs third law of motion is satisfied.
ÔÇ£DPM is valid up to around 12% by volume as particle volume and interaction isn't fully accounted for.ÔÇØ So in the case of the dense systems, should I increase the cell size (especially for the inflation layer) to avoid too high particle volume fraction?
Besides, should I try the DDPM model? Is it able to handle such large source terms?
• Rob
Ansys Employee
DDPM uses an Euler approach and may suffer from the same issues as you're adding the momentum terms manually. In dense flows particles shield one another (slip stream) so less particle momentum is transferred. This is why we have so many options in the Eulerian model for phase interactions.
• Felix_unsw
Subscriber
Thanks Rob. Are you saying that I should stick with my current model and treat those locallydense particles as granular, which have less momentum than individual particles?
BTW, the particles are dilute for the whole system. Because my model considers particle-particle and particle-wall interactions via DEM method (implemented via UDFs), some particles are deposited on the wall, resulting in a locally high volume fraction of particles to the cell.
• Rob
Ansys Employee
I think so: retain the models you have for DEM etc but review the literature on high volume fraction momentum transfer. It's another stage in your coding rather than a rewrite of any models.

• Felix_unsw
Subscriber
Got it, thank you very much for your help!
Actually, I do have another question if it's ok to post here: Is there any way to consider the effect of particle volume fraction on the flow in the CFD-DPM model? Or do I have to switch to Eulerian/DDPM to consider this effect?
Since I already know how to get the particle volume fraction for each cell, I can directly transfer it to the 2nd phase via UDFs in Eulerian or DDPM model, so the fluent can then take this effect. However, I can't find where I should transfer this parameter in CFD-DPM. May I have your advice?
• Rob
Ansys Employee
If the solution is coupled (interaction with continuous phase is ON) the amount of particles will effect the flow. If you mean you want to add the particle volume into the flow then that's where the Eulerian models come in.
If you want to start adding in Euler mass you will need phase source terms and then will need to deal with some forces etc being included by Fluent and the UDF. That may not be easy to untangle.
• Felix_unsw
Subscriber
Hi Rob, many thanks for your kindness. Now I have switched my model to multiphase-VOF model as I need to consider the effect of particle volume on the flow (related N-S equations are attached). In this model, I assume that the 2nd phase represents particles, so the particle volume fraction (╬Á) will transfer to 2nd phase via UDFs. Is this treatment reasonable?
Another question is whether the UDFs of C_U, C_V and C_W(c,tc) return the velocity of the mixed-phase in the cell? If so, do you know which UDF I can use to get the cell information for the specific phase (e.g., I only want to get the velocity of 1st phase in the cell)?

• Rob
Ansys Employee
VOF requires that you track each droplet, and resolve the mesh to that level. Mixture model and Eulerian allow you to track a dispersed phase with granular properties but the underlying physics is a little different.
• DrAmine
Ansys Employee
The cell thread is for Eulerian the phase level and for mixture or VOF the mixture thread level so all depends on how may many set of momentum conservation Equations you are considering.