[Pugnax]

I have a modeling question that I need some help with that I simply cannot wrap my head around on how to approach it. I am modeling the mass flow rate, pressure drop, and mass transfer rates of a rotating zigzag bed (RZB). A RZB is a “higee” distillation column; similar to say a spinning cone column, or a rotating packed bed. Attached is a picture of a simplified RZB geometry. In practice, liquid is fed into the center eye and the rotating bottom plate flings the liquid outward and up the rotating baffles. The baffles have holes/perforations halfway up which allow the liquid to “spray” onto the stationary baffles. The liquid then falls back down to the rotating plate and baffles and is repeated until it is flung out of the zigzag bed and collects down below. As liquid is being flung outwards, vapor is flowing counter currently through the zigzag bed and interacts with the spray that is coming from the perforations on the rotating baffles. This vapor exits through the center eye.

My thinking, as of now, is that I will use the inhomogeneous, Free Surface Model with air and water. I’m only modeling a 4-degree section of the bed using transient analysis. I believe the inhomogeneous free surface model is the most appropriate because there are distinct regions in the bed (i.e. on the rotating plate) where water and air are clearly separated. Entrainment of air in water occurs as water flung through the perforations. Water will be the continuous phase and Air the dispersed phase. The buoyancy ref density is set for Air, the bottom plate is rotating at 1000 [rev min^-1], and the reference pressure is set at 0 [pa]. Free surface model is standard, isothermal, homogenous turbulence, and density difference for both water and air. I have a mass flow inlet and an opening at the top and bottom set at 0 [pa].

My question is does this all seem reasonable? Is this an appropriate method to approach this problem or am I making horrible mistake that will lead to misery? I am planning on using CFX but also have access to Fluent but am not as comfortable using Fluent as I am with CFX. Would this geometry be better performed using the VOF model in Fluent? This analysis has my head spinning because it has both fine spray that would be nice to use particle models but it also is largely a free surface model. Any help or suggestions would be greatly appreciated.

[ghorrocks]

Thanks for the good description of what you are doing. I wish more people would post with useful information like that, it means we can have a more meaningful discussion.

Inhomogeneous free surface sounds like a good place to start.

Set the reference pressure to a representative absolute pressure in the domain, not zero. You have set up zero reference pressure and zero pressure at some openings - do you really want zero absolute pressure at the opening?

I cannot say whether Fluent will be better than CFX. Try them both and see which works best, or just go with the one you are familiar with.

[Pugnax]

Thanks ghorrocks! I appreciate the reply. You're right, I need to change the reference pressure. Ideally, this distillation bed would operate with a slight vacuum pulled on the vapor outlet at the center eye. I set the reference pressure to 1 [atm] and the vapor outlet at -101220 [pa] and the outlet at the bottom to 0 [pa]. I will try with CFX first and see if I can get some good initial results.

[Pugnax]

I am having trouble getting this simulation to converge and I believe it is because of my initial conditions and/or my boundary conditions. I set the reference pressure to 1 [atm] and the two openings to 0 [pa] . Since this is only a 4 degree section the mass flow inlet is 0.000333 [kg s^-1]. When I run the simulation and check the first timestep everything looks good. You can view the pressure contours in the attached image. The hydrostatic pressure looks right and the volume fractions are initiated correctly as well (the first image is 0.trn). After the first iteration the pressure skyrockets to an impossible level and stays that way until the simulation crashes; usually anywhere between 20 and 40 depending on my timestep. The second image is 1.trn. I've also included my expressions that I use for volume fractions and pressure in my global initialization. In addition, the timestep I have to use in order to keep the problem from crashing is prohibitively small (between 1e-7 and 1e-10) which again makes me think that I have poorly set or have an error in my initialization or my boundary conditions. "HydroP" is used as the Relative Pressure and "waterVF" and "1-waterVF" are used as the volume fractions for water and air in the global initialization, respectively. I cannot seem to find my mistake. Is there anything I am missing that could also contribute to such a dramatic increase in pressure?

EXPRESSIONS:
DenH = (DenWater - DenRef)
DenRef = 1.185 [kg m^-3]
DenWater = 997 [kg m^-3]
HydroP = DenH*g*(waterHt-z)*waterVF
myRotationSpeed = 1000 [rev min^-1]
waterHt = 0.0851 [m]
waterVF = if(z<waterHt,1,0)*if(z>0.00205[m],1,0)*if(x<0.0079[m],1,0)*if(x>-0.0079[m],1,0)
END

[ghorrocks]

Yes, there appears to be something fundamentally wrong with your setup.

Please attach your CCL and a drawing showing what you are intending to model.

[Pugnax]

I am modeling a Rotating Zigzag Bed by using a 4 degree slice of a full, 360 degree, circular bed using the inhomogeneous, free surface model, using air and water. There are two domains; a rotating one and a stationary domain. The slice is set up so that the two domains have rotational periodicity on each side and separate R and Z, GGI, transient rotor stator, zero pitch, interfaces between the domains.

The bed has three boundary conditions and operates at 1 [atm]. A mass flow inlet fed water at 0.000333 [kg/s] with two pressure and direction openings set at atmospheric conditions. The simulation is initialized with water filling the inlet and everywhere is air.

I am running the simulation with double precision, in parallel using, METiS, with transient rotor stator multipass and coupled partitioning.

By modeling this geometry, it is my goal to determine the overall flow, pressure drop across the bed, and flow rates through each rotating baffle. Eventually I would like to determine gas hold up, mass transfer, and model multicomponent flow (i.e. methanol and water, ethanol and water).

I've attached my CCL and an image showing the over geometry including openings and inlets. The highlighted area is the rotating domain and the rest is stationary.

Thank you for any insight. This model has really stumped me.

[ghorrocks]

Some comments:

You say you have a rotating domain and a stationary domain. What bit rotates and what is stationary?

You have activated a surface tension model. Are you sure you need this. This will make the simulation MUCH harder to solve.

Have you tried coupled volume fraction equations? OH, I see you have already activated that. Have you tried it without it?

You are using second order time differencing and high res advection scheme. I would make that first order and upwind while you are doing the development. Once the model is working as expected you can go back to your accurate but unstable schemes.

[Pugnax]

Thank you for spending your time to look at this. I really appreciate it.

In my previous post I included a picture of the geometry. In that image the highlighted green section is the rotating part and the rest of the wireframe represents the stationary part.

I have tried Upwind and first order with no improvement. I have also tried simulating with and without Coupled Volume Fractions and find that it being activated helps convergence somewhat.

I have just now tried simulating without modeling surface tension and it did not provide me with any improvement. The pressure still skyrockets after the first iteration. However you bring up a good point; I don't need the surface tension model for my initial runs. I would like to include it later but it helps to have it turned off.

I am thinking maybe it's my mesh quality. The mesh statistics show that overall i have very good quality but the areas of very poor elements is almost exclusively confined to the inlet section of the model. The inlet has a very hard angle (4 degrees) and it is causing very, very poor quality elements. To more specific, I have 450 elements with a Orthogonal Quality of 0.06 all aligned on the far left edge of the inlet. I am thinking that because everything is initialized from that area of the geometry it may be causing bad initial results that the simulation simply cannot recover from.

[ghorrocks]

I do not see anything which looks like a rotating domain. Why can't you put your green surfaces in a single stationary domain and put a tangential velocity on them? Then everything will be in one domain and considerably simplified. Or have I misinterpreted your drawing?

I would also recommend testing this model using a homogeneous free surface model initially and getting that working. Then do a dispersed air model and get that working. Only once you can successfully model the two types of air phase would I combine them together.