Learning Forum

[simon.schiffer]

I am using ANSYS 2026 R1 for my project. In my project, I am trying to compare a practical settling test with an ANSYS simulation. I am not satisfied with my current simulation results (because there are many more particles in the outlet in my practical experiment), so I would appreciate any suggestions for optimization. 

The settling tank has the following dimensions: height = 1.3 m / width = 1.8 m / length = 3 m

The inlet and outlet have a diameter of 100 mm

My test material consists of polystyrene particles with a diameter of 0.4–0.7 mm (assumed to be 0.6 mm) and a density of approximately 1040 kg/m³

In my experiment, I set the flow rate to 1.5 L/s and add the test material (1kg polysterene) .

After 10 minutes, my experiment ends, and I check the residue collected in the drain.

 

The following shows my simulation settings so far:

 

[Rob]

The model set up looks OK but you may need rethink the approach. 

What volume fraction are you expecting during the injection period? 1.5 l/s water is 1.5kg/s so with 1kg/s of a material that's near enough the same density your volume fraction is equal to the mass fraction of 40%; how does that compare to the DPM recommended range? 

The particles are slightly denser than water, so I assume they sink? You did include gravity? If they settle what volume fraction do you expect in the domain, and how are you accounting for packing? 

Why is the model base green? By default walls are black (foreground). 

 

[simon.schiffer]

Thanks for the quick reply.

So, should I set the injection time to 10 seconds (Start time: 0 and Stop time: 10s) to lower the mass fraction?

I included gravity. And yes, the density is very close to that of water, which is why the real-world experiment shows that some particles do not settle due to surface tension and flow directly into the outflow.
Can this behavior be modeled by only using DPM, or would I need to use a VOF as well? (I would prefer only DPM, because I only have limited claculating ressources).

(I think the green Parts show the changed Boundary conditions)

[Rob]

What surface tension? DPM particles won't see the VOF free surface other than there being a change in density & viscosity. 

If you change the injection rate that's fine, but you then change the flow dynamics. 

[simon.schiffer]

So it is not possible to explicitly account for the surface tension of water when modeling particle settling behavior using a DPM.

Which model should I use in Ansys if I want to take the surface tension of water into account?

[Rob]

Assuming you mean the phenomena that allows denser particles to sit on (or stick below) the free surface then, no, there is no default model in Fluent for that. It's also somewhat more complicated to code one using UDFs as you'll need to identify the cell with the free surface to then figure out the normal to add in the force to act on the DPM particles. It's doable, but not simple. VOF & DPM would be the starting point as the VOF model does have surface tension effects for the fluid pair (eg gas & liquid). 

There is a new option in Rocky, https://ansyshelp.ansys.com/public/account/secured?returnurl=/Views/Secured/corp/v261/en/dem_cfd_coupling/fluid-phase-calculation.html?q=vof which MIGHT give you more options. That will also require user coding, but would allow particle interactions, such as powder build up.