Error: Fluent - EDEM oupled simulation

Kiran Purushothama Keshavan

Hi,

I executed a coupled simulation for a simple EDEM-Fluent case, the simulation ran for 1011 iterations and it terminated because of divergence.

Please give me your comments on what might have gone wrong. I had previosly executed the EDEM and fluent case seperately and there were no errors.

I have included a few plots and the console data as attachments below.

Please advice.

Regards,
Kiran

Stephen Cole

Hi Kiran,

Divergence would typically be caused by the time-step or the particle size relative to the mesh size.

If it is time-step related I'd recommend reducing the Fluent time-step and/or the ratio between EDEM and Fluent in terms of the time-steps.

For the mesh size if an EDEM particle enters a fluent mesh cell where the particle is larger than the cell then this could cause stability problems in Fluent.  This would require a mesh change or consider reducing the under-relaxation factors for momentum and volume fraction transfer.

 

Regards

Stephen

Kiran Purushothama Keshavan

Hi Stephen,

I have EDEM time step at 20%, and then the Fluent time step is 50 times that of the EDEM time step, and still I get divergence very early in the simulation.

My particle is 1mm in diameter (5e-10 m3) while the smallest mesh element volume is 9.82e-9m3.

I missed trying with low relaxation factors for volume fractions.
I'll let you know how thus goes.

Thanks,
Kiran

Stephen Cole

Kiran Purushothama Keshavan said:

Hi Stephen,

I have EDEM time step at 20%, and then the Fluent time step is 50 times that of the EDEM time step, and still I get divergence very early in the simulation.

My particle is 1mm in diameter (5e-10 m3) while the smallest mesh element volume is 9.82e-9m3.

I missed trying with low relaxation factors for volume fractions.
I'll let you know how thus goes.

Thanks,
Kiran

Hi Kiran,

Relaxation factors should help but always worth while considering this does mean the solution takes longer to converge.

On the time-step it's worth considering the time-step value in EDEM, the % value is easy to set but always worth knowing what the value is in seconds so you can estimate distance travelled per time-step.

For example if your mesh volume is around 1e-8 m3 we could estimate that if this was a cube it's dimensions are around 2 mm (should be able to confirm mesh dimensions in Fluent).  If the particle is moving at 10 m/s (max velocity from your vectors?) then it would take 2e-4 s to pass through the cell.  For stability maybe have the particle in the cell for 3 time-steps which would be ~7e-5 s.

So best to consider the actual value of the time-step in EDEM and Fluent, if in Fluent the time-step value is greater than this 7e-5 s value Fluent would 'see' a particle jumping from cell to cell without passing through, which would not help with the solver stability.

Regards

Stephen

 

 

 

Kiran Purushothama Keshavan

Hi Stephen,

This makes so much sense. 

Thanks for pointing to this out. I'll keep you posted on my simulation.

Regards,

Kiran

Kiran Purushothama Keshavan

Hey Stephen,

So if the fluent mesh is 10x or 20x the particle size, then when we run a coupled simulation let's consider the particles accumulate at the bottom of the geometry so since the particles occupy a fluid volume in fluent, can there be a layer by layer accumulation? 

1. What I'm essentially asking is if a fluid volume (bigger than DEM particles) has multiple particles, how would fluent read this data compared to when the fluid volume only contains 1 particle in the fluid volume.

2. Let's say the small particles fall into the finite volume and fill up the space, and multiple other particles stack over each other, then would it be better if I post process this data to visualise on EDEM or Fluent?

I do not want to loose the info when it comes to the coupled fluid flow influence on individual particles as a compromise to mesh cell size.

Please advice.

Regards,
Kiran

Stephen Cole

Kiran Purushothama Keshavan said:

Hey Stephen,

So if the fluent mesh is 10x or 20x the particle size, then when we run a coupled simulation let's consider the particles accumulate at the bottom of the geometry so since the particles occupy a fluid volume in fluent, can there be a layer by layer accumulation? 

1. What I'm essentially asking is if a fluid volume (bigger than DEM particles) has multiple particles, how would fluent read this data compared to when the fluid volume only contains 1 particle in the fluid volume.

2. Let's say the small particles fall into the finite volume and fill up the space, and multiple other particles stack over each other, then would it be better if I post process this data to visualise on EDEM or Fluent?

I do not want to loose the info when it comes to the coupled fluid flow influence on individual particles as a compromise to mesh cell size.

Please advice.

Regards,
Kiran

Hi Kiran,

For point 1 Fluent only sees a volume fraction of particles in the cell, so if you have multiple particles it's the sum of the particle volume in the cells which Fluent sees when calculating the drag.

 

With regard to visualisation a mix is often best, EDEM will give you more data on the particles and you can use more tools like bin groups to look at concentrations in different areas.

Regards

Stephen