I'm familiarizing myself with Fluent's VOF capabilities. As a test problem I'm looking at an air bubble (radius = 1") rising in a cylindrical column of water (radius=6", height=24") in a normal gravity environment. The problem is being solved axisymmetrically. The material properties are Fluent defaults for both phases and the only interaction is surface tension. The pressure discretization is done with PRESTO Momentum advection terms are handled with MUSCL SIMPLE for the pressure velocity coupling with default relaxation parameters for all the variables. Per Fluent recommendations, air is the primary phase. The initial location of the reference pressure is in the center of the air bubble. The momentum equations are solved implicitly.
As the bubble rises, the reference pressure location is eventually in the heavier phase.
I tried several approaches: 1. As a baseline VOF equation solved explicitly with geo-reconstruct algorithm. Initially the solution looked OK but after marching out a second, the interface is extremely corrupted. Instead of a single bubble I get multiple smaller bubbles. A plot of the density field reveals the minimum density in the domain has increased from 1.225 to about 26. Since the two phases are incompressible nothing should happen.
2. Looked at several different time steps - as expected the larger the time step the more corrupted the solution becomes. Surprisingly, when I decreased the timestep by an order of mangnitude the initial solution (100 time steps to get to 0.1 s) was much worse than the case outlined above (10 time steps to get to 0.1 s).
3. Tried running VOF implicitly with high resolution interface capturing but had a hard time getting a solution. The residuals eventually stagnated. Decreasing the time step just delays the point at which residual stagnation occurs.
4. Tried adaptively refining the mesh around the phase boundary but this didn't help much.
5. Tried the compressible VOF scheme (air density is modeled using ideal gas law) with floating operating pressure. With fixed operating pressure the convergence behavior was very poor and I killed the simulation before reaching the first time step. By floating the operating pressure I got a solution similar to #2 but I'm still not sure the floating operating pressure routine is being implemented correctly. From what I gather, the method just rescales the static pressure field instead of updating the pressure through thermodynamic or mass conservation considerations. Regardless, even though the solution was qualitatively similar to #2, the mass loss of the bubble was about an order of magnitude larger. I gather this is because the density floated with the pressure. Since there's no mass transfer between the phases, the density and volume of the air bubble should remain constant during the simulations.
6. I ran the case in zero gravity just to get an idea of what the spurious velocities were. And while they were larger than what I expected, I don't think they're large enough to corrupt the solution as much as I'm seeing.
Any help would be appreciated. Steve
Re: Fluent VOF
Re: Fluent VOF
Maybe I am a complete idiot, but I simply do not see how this paper has anything to do with the subject, other then "bubbles"!? This paper does not use Fluent's VOF capability and has absolutely no connection to any interface-capturing methods (as VOF is) whatsoever, and although after a 5 minutes read, it does look like an interface-tracking method, I am still not fully convinced. I have to read it more carefully.
About Steve's problems:
- first of all, that reference point for pressure is extremely important, so I would suggest you to modify your case to include an air layer at the top of the column and put the reference point there;
- second, although the Fluent Doc is recommending PRESTO scheme for pressure discretisation with VOF, from my experience I found that Body Force Weighted scheme is much more reliable and stable;
- third, I had bad experience with using symmetry BC in narrow spaces (like a column) because they heavily altered the solution, so I would strongly recommend you to try your simulation in a 2D plane space instead of 2D axisymmetric, with no symmetry BC at the middle;
- fourth, you should not use anything else but explicit VOF, with geometric reconstruction of the interface, and be very careful about the timestep, not to heavily exceed CFL=1 at the interface (a CFL= of 2.5-3 is still acceptable, but you'd better not exceed 1).
I hope this will be helpful.
All the best,
Re: Fluent VOF
Thanks for the advice. A few more things I've tried:
Instead of PRESTO I used Body-force weighted for pressure - the residuals stagnated after a few time steps so I killed the job.
I agree the reference pressure location is important. I created an layer of air at the top of the water column and set the reference pressure location somewhere in the air layer. Throughout the simulation, the point remained in the lighter phase. The improvement was only marginal. Significant interfacial degredation occurred.
My CFL number is set to 0.25.
Modifying the job to be 2D instead of axi- is doable for this example problem. Unfornately the problem I'm really interested in solving must be done 3D or axi-. The computational time associated with a 3D simulation is high so I need the axisymmetric simulation to work.
I tried computing the body force explicitly but again there was only a marginal difference between this and the original solution.
To make sure the mesh wasn't an issue, I quadrupled the grid density to ~60000 cells by adapting the entire liquid column. Comparing the solution after a few seconds of simulation time, the interface was a lot messier than in the original solution.
I thought the problem might be that the density ratio is too high. To investigate this further, I modified the material properties. Instead of 1000:1 density ratio, in the lighter phase, I set the density to 1. In the heavier phase, I set the density to 10. The viscosity in both phases was equal. The interface was severely degraded. The solution was much worse than the original.
Right now I'm really at loss on how to proceed.
Re: Fluent VOF
I was really intrigued by this problem, so I decided to try it myself. I must say that I didn't have any problem at all, the simulation converges even for the axisymmetric domain. Of course, the bubble behaviour is different in 2d from 2d axisymmetric, but they both run smoothly to the end. And I only used 8000 cells for the axisymmetric problem!
I realised that I forgot to mention some very important steps, needed to ensure the success of such a simulation:
- surface tension must be specified (a typical value would be 0.072 N/m);
- before marking the cells registers that will be used for patching the phases, it would be a good idea to use this scheme command: (rpsetvar 'patch/vof? #t); this way you will be able to get a nice and smooth interface right from the patching step;
- the time step must be small enough to guarantee a CFL<1 near the interface (that is the CFL I was talking about, not the CFL=0.25 from the Define/Models/Multiphase/VOF GUI panel!); a value of 0.001 s should be enough for most situations.
I also have to mention that although the axisymmetric simulation should be closer to the reality than the 2d one, in the case of big bubbles (which is pretty much everything above 1 cm) that eventually brake into smaller bubbles, the axisymmetric solution is again far from the truth. But at least up to the moment when the big bubble brakes, the solution remains physical.
If you like so, I could send you the .cas&.dat files to compare with your own.
All the best,
could send me the case/data to me ? i want to compare with my own.
all the best.
High viscous ratio liquid, VOF
I am modeling the coalescence of 2 films using the VOF scheme with Geo-construct wth Ansys Fluent. The films are surrounded by air. So far the simulations with lower viscous liquids (<1Pas) were running fine.
But I need to simulate a highly viscous liquid (>50Pas) and the solution is diverging. I tried the CISCAM scheme for interface tracking but it still seems to diverge. The flat interface is breaking and forming drops, which is definitely looks odd. It seems to do this even at very low time steps.
I also checked if it was an issue with the mesh, but the same issue repeats with a finer mesh.
This issue seems similar to the issue described above.
How was the issue finally resolved?
the problem of continuity convergence in transient VOF multiphase model?
Currently, I am using VOF model to simulate water and oil flow in a pipe. My regime is dispersed flow and Weber number is so high that I did not consider the effect of surface tension. I put residual for continuity as 0.0001 and for velocity components as 0.001 as well. I have the problem of convergences of continuity, since I am solving Transient, in different time step continuity remained constant while residuals for velocity are converged. I reduced URF, again problem exist. How can I solve this problem?I attached you residuals.
|All times are GMT -4. The time now is 18:13.|