Learning Forum

[gerald.gallagher]

Hi,

I am attempting to simulate a sphere settling under gravity in a viscous fluid (water for now) using the Macroscopic Particle Method (MPM) in Fluent 2023 R1.

I managed to set up a sphere falling in air by watching a good video posted on a YouTube channel mentioned in the CFD Online thread https://www.cfd-online.com/Forums/fluent/33104-macroscopic-particle-model-mpm.html:

https://youtu.be/bGU62t9DDy0

I tried to set up spheres falling in water with steps from another video posted on the same YouTube channel:

https://youtu.be/920ajl_nV68

However, the spheres either don't move or the behaviour is unphysical. Also, the continuity residuals are very large. The geometry I use is very similar; it is slightly simplified to be just a rectangular box without the reduction in size in the middle of the domain, but uses the same overall dimensions from the video. The mesh I am using has very similarly sized tetrahedral elements as well. I am following the steps as closely as possible, but I still cannot replicate the behaviour from the video.

I should note that I had to replace the animation setup from the videos with the more current "scene" setup.

Would anybody have any advice on this issue?

Thanks!

[Rob]

What material is the MPM particle defined as? 

[gerald.gallagher]

Hi Rob,

Thanks for your reply.

I set the particle density to 1100 kg/m3 and diameter as 0.02 m in the MPM setup window as per the video. In the standard Fluent Materials section, "aluminium" is set as the material for "Solid" and I change the density to 1100 kg/m3 as per the video. The material "anthracite" is set as the material for "Inert Particle" and I change the density there to 1100 kg/m3 as per the video.

It did seem strange that I should have to change the density in multiple places to the density of the particle. Is there anything that I am doing incorrectly?

Thanks

[Rob]

I've not used the model since it was a UDF function: it has a use but for dropping objects we tend to favour moving mesh or DEM now. I suspect the DPM part is because of the way the model works, no idea about why you'd need to alter the solid material. 

[gerald.gallagher]

 

Thanks Rob. Over the past few weeks I managed to get better MPM model results using a smaller time step. I am testing MPM models with hexahedral meshes at the moment and the results are also good. In relation to simulating a dropping object using moving meshes, is there literature or any tutorial with advice on setting up 3D dynamic mesh 6dof simulations that don’t use the VOF multiphase model and involve geometries moving (ideally falling) in a viscous fluid? My interest is primarily in relation to hexahedral meshes, and so far I understand that hexahedral meshes can only be layered and/or smoothed, but not remeshed. Thanks for your time.

 

[Rob]

That's pretty much it. Full remeshing in hex isn't possible. One trick is to move a block of mesh around the object and layer above & below that. 

If you follow the guidelines for things falling into VOF and just omit that step it should be fine. We often make tutorials/examples a little more complex as it's then possible to cover multiple topics in one example. 

[gerald.gallagher]

Thanks Rob. That's very useful information in relation to the hexahedral mesh, I'll investigate that. I managed to run a tetrahedral-based dynamic mesh 6dof version of my MPM simulation without the VOF model turned on and I obtained good results. I just had to add the calculated buoyancy force directly in the UDF using prop[SDOF_LOAD_F_X]. Would the recommentation for situations like this be to stay with tetrahedral meshes, or should I not have any major issues using hexahedral cells? Thanks again for your time.

[Rob]

I think the solver will deal with the buoyancy effects automatically - there's a reason we add mass to the 6DOF model! 

The best option for cell type tends to depend on what you want to know, and how you're modelling it. One approach that does work well is to drop the object with a fixed mesh around it and remesh further away: that means there's no remeshing around the object of interest and you can use inflation. 

[gerald.gallagher]

 

That makes a lot of sense, thanks. I had assumed that the solver should automatically handle buoyancy effects like you say, but without modifying the UDF, my results were quite inaccurate even with increasing mesh density. I followed the advice of users in the thread https://www.cfd-online.com/Forums/fluent/105250-buoyancy-6dof-solver-fluent.html and while I want to run a few more tests, the results are much better. Perhaps I missed something small in the case setup which would avoid the UDF modification?

 

[Rob]

 

There have been a few changes in the way 6DOF works, so you may find older information sources are less reliable. Check the lifeboat launch in the Fluent Help guide. 

Edit - we think buoyancy is accounted for by default. But please check, I don't tend to model moving mesh, and the moving mesh specialists tend not to do much multiphase work! 

 

[gerald.gallagher]

No problem, I'll do more reading based on your suggestions and will keep testing. Thanks for taking the time to answer my questions!

[Mepal]

Hello Gerald,

I used to create large particle by using MPM technique.

Last year, around July 2022, I followed all tutorials you sent in your comment. Yes, the particles did not move in some cases. I fixed it by doing some setting in MPM setup,then the particle moved.

However, I by heart cannot remember which setting I did. But the key is in MPM setup. Hope this help.