erratic and unexpected particle velocities

Submitted by evansmuts on Tue, 08/28/2012 - 14:45

Hi

I am getting strange behaviour of my simulations that seem to be very mesh dependent. Can anyone please give some insight? Sorry for the long post, but I have tried to give as much information as I can.

My model uses coupled CFD-DEM (cfdemPisoSolver v2.3 with model "A") for small particles (>10 microns). The domain is a small box. The fluid is water, and the particles are 6 times denser than water. Fluid starts at zero velocity, but is given motion from a translating wall on one face of the box. For these results here the particle are not entirely at rest - after inserting the particles I run LIGGGHTS for 1000 000 iterations with no gravity to let the simulation settle. Then I run the coupling.

I measure the force on the translating wall from both CFD and DEM (basic wall). I then combine them to calculate the shearing force on that surface. After multiplying by a conversion factor, I get the shear stress. So the shear stress behaviour shown in the graph (attached) is very much related to the wall force.

The graph shows shear stress (particle and fluid forces) vs shear rate (essentially speed of the wall). I expect the values to lie somewhere between the "pureCFD" line and the "experimental" curve (similar to the den1 curve). I have given results for 3 different simulations, each with a different mesh density. Cell size: "den1" cell = 4.1 times particle diameters, "den2" cell = 2.8 particle diameters, "den3" cell = 2.0 particle diameters.

In this graph the behaviour of the curves is dominated by the DEM forces, which are about an order of magnitude higher than the CFD forces. From visualising the flow, the erratic force behaviour seems to be a result of certain particles having a much higher velocity than the rest (resulting in a bigger force on the wall). What I don't understand is why a finer mesh (den3) gives a more erratic behaviour of the particles/flow? From single particle tests of a particle impacting a wall, the finer mesh gives a much better resolution of the particle movement. The coarser mesh obviously diffuses the flow, which probably causes the smoother change in the forces. I have attached a fluid velocity plot (cut and vectors) for the coarse mesh to illustrate the pockets of high velocity flow (due to high particle velocity). In this plot some of the particle velocities are double the flow velocity (not shown).

I must point out that these results were taken for a coupling interval of 250. Running with smaller intervals gives much more erratic behaviour.

According to these simulations, a coarse mesh and big coupling intervals give "better" results. This is the opposite trend to what I would expect!!

I am also wondering if the DEM timestep is too large. Using "check/timestep/gran", I find that my DEM timesteps are 30% of Rayleigh time and 2% Hertz time at the beginning of my coupled run. Could this be a cause of the high velocities experienced by some particles?

Any insights/comments would be appreciated. Thanks.
Evan

Forums:

Maryam | Fri, 11/16/2012 - 23:53

I am also running a simulation with similar particle size. I am not sure about the grid size effect but I also see very large velocities and on the CFD side, spikes of very large (positive and negative) pressures which I guess is due to large particle velocities at the moment they bump into other particles.

Using a tiny time step (1^-10) and limiting Ksl helped to stabilize the solution (at least it does not blow up any more!) however, I still see those spikes. I'm wondering if using “fix nve/limit” would help or if implementing this fix makes any physical sense.

**update 1: Well, actually nve/limit didn't help! now I'm out of ideas!
**update 2: Increasing the number of grid cells (and hence dispersing the volume of particles over larger number of cells) reduced the crazy peaks of the spikes a lot

In my model, fluid along with the small particles flow over a very dense packing of frozen large particles, so at some cells local fluid velocity gets very large, this also adds to the stability problem in my opinion.

Maryam

evansmuts | Mon, 11/19/2012 - 15:32

Hi Maryam

Thanks for those ideas. I didn't think of trying nve/limit, though I see you say it doesn't work. I don't like the idea of limiting Ksl as that is like "cheating" to get the model to work when there must problem in the setup.

I found that using larger CFD cells made the simulation more stable, but I still got the high velocity spikes in places. After, talking to Chris Goniva, I decided to use a CFD cell size that is ~4 particle diameters along each edge. Anything smaller than this and you could end up with a situation where the cell has little or no fluid in it, which will cause problems for the CFD.

In your case, a smaller CFD cell would resolve the fluid flow more accurately, which may improve the smoothness of your result. But there is a limit as I mentioned above.

What coupling interval do you use? I use 100, which is more stable - anything smaller gives bigger fluctuations.

After talking to other people in the field, they suggested I reduce particle stiffness (< 3 orders of magnitude) so you can increase my timestep size but still have valid Rayleigh time criteria. Therefore you can get comparable results for a bigger timestep.

This did not reduce the high velocities for me, but a smaller particle stiffness may help in your case...

I hope this helps you?

Regards
Evan

Maryam | Wed, 11/21/2012 - 23:21

Hi Evan,

Thanks for the update. Actually I did a lot of experimentation and I am still trying different tricks. Here is what I experienced during numerous runs:

- My perception is that small coupling interval does not allow the CFD simulation to get stable before it sends correctly updated velocity information to the DEM solver. I increased my coupling interval 1000 times and now the spikes are almost gone.

- In my case, Ksl must be limited, otherwise, particle velocity governs the fluid flow, so when they bounce back, they carry the fluid with them (even change the direction of flow), which does not make any physical sense and causes stability problems

- For the configuration of my problem, large CFD cells results in high Courant numbers and divergence on the CFD side. Perhaps a combination of large cells and small CFD time-step can rectify the divergence problem, have not tested it.

- I used the extremely small time-step for a low stiffness case! As I said it did not remedy the spike problem. I used that time-step to prevent losing particles. It helped but the main reason of losing particles was large velocities coming from a non-stabilized flow solution due to small coupling interval. With larger coupling interval, I could increase my time-steps back to 10^-8. I still suffer from losing particles but at this moment have not checked if they are exiting the other end of the domain or simply lost during an impact. Also, for some cases, the CFD solver blows up which I believe is due to pressure BC (to represent pressure driven flow)

Sorry for the long description. I believe the problem that I am working on is dominated by fluid flow, so it makes sense to decrease the Ksl or even try one-way simulation (which I haven't tried yet)

Best regards
Maryam

Maryam

cgoniva's picture

cgoniva | Tue, 12/04/2012 - 13:44

Hi,

I suppose your calculation of the fluid is incompressible?
It might help to stabilize the solution to use pressure=0 as reference (in the BCs) instead of 1e5, especially if pressure gradients are small this will help a little.

Cheers,
Chris

Somnath | Tue, 12/04/2012 - 22:24

Hi,

Do new particles cross into your CFD domain as the simulation progresses? I am also getting spikes in pressure when there is a stream of particles (fix insert/stream) crossing the boundaries and entering the CFD domain. On the other hand if I create all the particles inside the CFD domain before beginning the simulation and just stick to them, the spikes are not there.

Regards
Som

Maryam | Tue, 12/18/2012 - 02:52

Thanks Chris, I tried zeroing out the BC. It actually didn't eliminate the spikes; however, the main problem is due to my very high volume fractions. When I omit the drag force model in the couplingProperties file, the run goes smoothly. I still need to understand the physical meanings of those drag force terms.

Som, I see those spikes even when I have flow over frozen, fixed particles!

Maryam

evansmuts | Fri, 12/21/2012 - 15:31

Hi Maryam

Thanks for all your replies. I just got back now after being away for two weeks, so I am only replying now.

For me, a coupling interval of 500 or 1000 is VERY unstable and the simulation crashes soon after starting. A bigger coupling interval should theoretically allow the particles more time to accelerate and match the fluid velocity. But it would also mean larger "jumps" in the fluid velocity in an unsteady flow, which would mean larger changes to the drag force (because it updates force calculation at larger/longer intervals), and possibly larger velocity spikes. Does your simulation reach a "steady-state" or is it completely unsteady over time?

I see your point about limiting Ksl, but it also seems "unphysical" to limit this value too much. In my case, limiting ksl does not make much difference. You said you have high volume fractions, what is the range you are looking at? I think limiting Ksl would be more important at high volume fractions. What are the densities of your fluid and particles?

While talking to Chris (Goniva), he suggested I try increase the number of nCorrectors in the PISO algorithm (>4) to give the pressure field a chance to settle. I am busy testing this, but it's too early to say what difference it will make. I will let you know the results of these tests.

Cheers
Evan

Maryam | Tue, 12/25/2012 - 03:12

Thanks Evan,
I'd appreciate if you share the results of your tests.
I have to admit that I used the tools somehow blindly, the volume fractions I used were as high as about 70%-80%. The whole simulation is not steady state; however, I don't expect large fluctuations, just slight decrease in flow rate over time.
I decreased the solid volume fraction and it became more and more stable (obviously!) I am now confident that for my extreme case, the available force models are not very useful. I might need to directly model the pore space to avoid high solid volume fractions.

Maryam

vinaym | Mon, 03/19/2018 - 17:08

What is the right way to determine an optimum Ksl limiting value? of course without affecting the simulations results a great deal .

Thanks and kind regards,

Vinay