Problems with multiphase tangential separator
 

Hello guys,
I have to model a tangential multiphase separator. I have a cylinder in which the inlet pipe enters tangentially, like in figure1. Gas phase exits at the top and liquid at bottom. I setted segregated flow and k-epsilon turbulence. In the phase interaction model I specified the drag force and the lift force as Tomyiama model.
The inlet is a velocity inlet and outlets are split-flow outlets. This is my first time working with cfd, so I havre surely done something wrong...the solution doesn't converge, as you can see in "mass-flow sum" figure and in residuals, but I don't know what to do...maybe I have to use a finer mesh.
Please help me!
Thank you so much
Attachment 38763

Attachment 38764

Attachment 38765

What are your y+ values?

Also, can you show some shots of your mesh?

I would recommend k-w, not k-e for this type of problem.

Thank you for the answer, but I solved this problem using a better mesh. So I think it was the problem. Now I'm using Reynolds stress turbulence and results are more realistic.

Still watch your y+ values. They are very important.

Ok I'm monitoring Y+ values. My highest value now is 170. Is it too high? What's an acceptable range for a turbulent flow (reynold is about 2,000,000)?

I have a trimmer mesh with Prism layer mesh added. The prism layer thickness is absolute 0.005 m (100% relative to base size) and the number of prism layer is 3. I tried with 10 prism layer, but the solution diverged. Can I solve the high y+ decreasing the base size of the mesh, or I have to do something more?

I would play with both layer thickness and number of layers to try to achieve both the y+ requirement but also the volume change requirement. That is probably why your 10 layer model diverged. The transition from your last prism layer to your core mesh was too aggressive. Try to make it so that the prism layer grows to meet your core cells, typically you would try to keep your volume change from cell to cell below 20%. You don’t need all 10 layers to be in the boundary layer, just the first 5 or so. The rest can just help you transition outward.

Without seeing your mesh it is hard to say what to change, but I would start by setting number of layers to between 7 and 10 and increasing the thickness to maybe 0.01m or even 0.015m.

Thank you very much, you're the best!
Last question: the inlet boundary is a velocity inlet: the pressure of the separator is 130 barg, but I don't know exactly pressure of top outlet and bottom outlet. Is it right to set both them as split flow outlets?

No, I would only do that if you already know what fraction of your flow rate is going through each one. The pressure of the separator, is that the pressure differential from inlet to outlet? If so, leave the pressure outlet as zero. This is like specifying atmoshperic pressure (or zero gauge) and since your inlet is specified in gauge you are all set! No need to convert that to gauge pressure.

No, 130 barg is the inlet pressure. The Top outlet pressure and the Bottom outlet pressure only depend on pressure drop. So I don't know the two outlet pressures...

So you know flow rate, but not the split in flow rate at the exit and not exit pressure? It seems like your problem isn't very well defined if you don't know what is happening at your boundaries.

Yes, I don't know the split in flow rate and the exit pressure...I do not have an experimental model, so it is very difficult to modeling...The only thing is to try every possibility and check the most reasonable...

Bummer. You might try the adjoint solver, it is made for this sort of thing. Look at the help docs, User Guide > Modeling Physics > Modeling Flow and Energy > Solving the Flow Adjoint.

You will still need some sort of criteria to judge against though. I assume you have some kind of performance perameter you are looking at that will determine your optimum or correct split, no? If you go this route, drop the pressure outlets and go with split flow outlet at your boundaries. Then the split ratio will be the variable that you feed into the adjoint solver. I haven't really used it beyond the tutorial so I won't be much help I am afraid.

Good Luck!

ok tank you very very much! You saved me!