Stability problem due to turbulent dispersion force in a subcooled boiling model
I am developping a Euler-Euler model for subcooled boiling. My starting point was the twoPhaseEulerFoam solver. My case is a simple 2D-channel.
I started to implement the adiabatic solver, with the different interfacial forces acting on bubbles (drag, lift, turbulent dispersion, virtual mass, wall lubrication), but without phase change at the interface nor nucleation at the heated wall. I tested this adiabatic model and it worked properly, i could observe the wall-peaking phenomenon that has been observed in the experiment.
So I added the boiling model proposed by Kurul and Podowski. And my program crashed after 0.007s. What happens is that close to the heated wall, there is a layer of cell for which the volumic turbulent dispersion force is tremendous (1e10) because the void fraction gradient (grad(alpha)) is huge, since alpha increases for near wall cells due to evaporation and is very small in the bulk (SUBCOOLED boiling).
To solve this problem, I tried to transfer the turbulent dispersion force to the pessure equation but it still crashed.
Then I used the limiter "cellLimited 1" for the gradient scheme used in grad(alpha). Now the solver does not crash as fast as before but I think that the limited values taken do not reflect properly the reality. For example I now observe very high lateral components on the volumic drag and turbulent dispersion that compensate each other (+ and - 200000). In comparison, the lateral wall lubrication value is about -2500. And my solver still crashed (after roughly 1s of simulation) because the void fraction reaches too high values in near-wall cells (higher than a limit fixed at 0.52 for nucleate boiling). I think this can be due to the weird turbulent and drag forces I got but I am not sure...
I would be very grateful if you can share idea or comment about my problem.
I am also troubled by this problem. I try some method, however the result is frustrate. One year later, have you solved the problem?
Sorry for the long delay, i was on vacation and came back yesterday.
Unfortunately, I did not succeed in implementing completely the nucleate boiling model. I worked 6 months on that project and at the end, I had a solver for adiabatic bubbly flows, but my diabatic solver did not give satisfying results. Other students/post-docs will continue and finish my work, as it was a part of a bigger project.
However, concerning this stability problem, taking the "cellLimited 1" gradient scheme for the void fraction, and removing the virtual mass force had solved it. I guess this should work in your case as well. Then the results were not quantitatively good but qualitatively OK, and the solver was stable and robust.
Let me know if this work for you too.
Thank you for your reply! Actually, I just worked 2 months on subcooled boiling. Now I have added energy equation, however the turbulent dispersion force has always trouble me. The information you supplied is of great help for me! I hope can watch progress of your project
I'm simulating a tube with water flow.
The tube encounters boiling near the wall.
I intend to calculate 'void fraction versus enthalpy' along the channel.
Can you help me how to calculate void fraction?
I'm in an emergency condition.
Waiting for your comments!!!
I hope you're using an updated or latest version of twoPhaseEulerFoam (last update May 25, 2011) or you went through to fix its them since there were bugs in the previous version...
Also, which model are you using for TD...I did implement FAD by Burns et al and I experienced the same instability. I implemented it in the 'older' version which contains bugs. I haven't given it a shot on the latest which I planned soon. I also notice that the instability was great for Gidaspow drag model. This is because there was bug in the implementation of this model:
lastly, the PISO based algorithm is known not to be stable. If you can change it to PIMPLE, then you'll be good. I known that Alberto claimed to implement this PIMPLE. Caution is required here since it's not included as standard solver and required a THOROUGH validations. Since you're modifying the solve, it might be probably worth a while to take a look at his version.
I hope this helps...
Thanks for your reply.
I'm using ANSYS CFX version 12 and 13.
I need to apply two phases, water and vapour. I encounter small nucleate boiling near the wall and intend to optimize it so that the system works in single phase.
I talked to my professor and he said ansys cannot work in these two phases. He said because of condensation and vapourization, cfx doesn't have the equations needed for this phase change.
Hope you can help me in this matter.
I haven't used neither CFX nor OF for modeling condensation or vaporisation. Ideally, there should no difference between them. You want to try this:
Check their manual/documentations to see what they actually have...They have a well-written documentations on their models and even state its limitations. If there's any particular model you're interested and missing you can implement it via USER defined subroutine or function.
Also, check their tutorials to see if they've a case similar to yours...on top of my mind will be Tutorial 26 (Axial Turbine Equilibrium ....)
Check their tutorial cases to see if you can have any case close to yours. Then access its capability and what's missing....The beauty of this code (software) is that you can google it and might get some examples or modifications which is close to your case. The downside is that you really need to take your time and go through it to see what it's doing and understand each line. Since most of them have not gone through quality assurance and might contains bugs. I can't think of any tutorial for OF but I bet cha, you aren't the first time working on this.
Check the latest version, OF-2.0.1(x)
Whether CFX or OF, you need to have some programming skills especially if what you're looking for isn't included in their standard package. CFX requires fortran whereas OF requires c++. Remember, the realty is that, our current knowledge of CFD on multi-phase or multi-component is still in infancy, and the accuracy and reliability of these codes shouldn't be taken wholeheartedly.
Feel free to message me if you've questions.....
|All times are GMT -4. The time now is 19:34.|