[SebastianSchuster]

Hello everybody,

I want to simulate flow through a nozzle. At the inlet I have liquid CO2 which evaporates in the nozzle.

I use the Peng-Robinsion equation of state.
At first I did a homogenous simulation and get an exit vapour volume fraction from 0.3. Based on this simulation I create an inhomogeneous simulation. Liquid CO2 as continuous phase and vapour CO2 as dispersed phase. To simulate boiling I use the "Thermal Phase Change Model".

I follow the modelling instructions in the CFX Help and set the Nusselt Number on the dispersed side to 1000 and on the continuous side set it to Ranz-Marshall Correlation.

The result of my simulation is that I have superheated liquid at the outlet of the nozzle and no vapour. During the simulation the liquid CO2 Temperature remains constant form inlet to outlet.

First I thought the liquid is not in thermodynamic equilibrium, so I set a very long tube at the nozzle outlet (50 times the length of the nozzle). Result is that liquid temperature at the outlet of the tube is still the same then at the inlet. Also there is no boiling in the tube.


At the moment I can not imagine where I did the mistake. So I hope somebody has experience with such simulation and can help me.

So if anybody knows about a mistake in my setup or about a general problem in the phase change model please tell me.


Best regards

Sebastian Schuster

[mscanlon74]

Sebastian, has anyone replied back to you on this question? Or did you receive some assistance from Ansys that may have helped you solve your issue? I'm running into a similiar problem with propane liquid being metered into a heat exchanger where flash evaporation is supposed to occur. I haven't been able to get the liquid propane volume fraction to change at all. I set up the model with an initialization of the propane coming in at 20 C and the heat exchanger domain set to a temperature of 90 C, but the heat transfer to the fluid does not seem to be as much as you'd expect it to, the propane temperature distribution is only differing by maybe 5 C. If you were able to resolve your model and have any advice, I would appreciate if you could possibly share that with me. Thanks in advance.

[SebastianSchuster]

Hello,
do you have an assumption for the bubble diameter. I had the problem that I assume to big bubbles. You can use the Weber number to calculate the bubble diameter at the nucleation point or use a nucleation model. Perhaps the implemented one in CFX is also fine for your problem. I think your working fluid starts to evaporate at the walls of the heat exchanger perhaps you could use one of the wall boiling models.

Best regards

Sebastian

[mscanlon74]

Sebastian, thank you for answering my post. To get the model going, I first chose an arbitrary bubble diameter of .005" and then I ran some models with the bubble diameter increased to .125". I'll look into your suggestion of trying the Weber number and see how that changes the set-up.

I've tried running the same set-up with the Wall Boiling method active and inactive, but mostly inactive. I plan to keep running this same basic model with some of the different options in use or not in use and try to evaluate what seems to give the results that converge the most.

One of the last models I ran, it appears that there is some phase change taking place from liquid to gas when I looked at the results in Post. I took this model and made a slightly different version and started to add more monitoring points during the solving process to track the temperatures of the 2 fluids and the solid domain that is supplying the majority of the heat transfer to the fluid. I can see a sharp temperature decrease in the gas after approximately 20 iterations and then it levels off the rest of the run.

This last model was running pretty good for about 186 iterations and then it crashed with an error message stating that there was a fatal overflow in the linear solver, a return code 1. I'm not exactly sure what that is telling me. The one thing that has had trouble converging during the solution is the fluid heat transfer and since that has a lot of influence on whether or not the phase change is taking place, I am not real confident in the solution yet.

[SebastianSchuster]

Hello,

the problem with the discreasing temperature is hard to solve without knowled of the whole setup. That the temperature remains constant my be caused by the table generation upper and lower temperature. I think you are using Redlich Kwong, Peng Robinson or rgp table. You could try increasing the table range.
Overflow in the linear solve can often happen in two phase flow simulation, but the reason for it is strongly problem dependend. Most often the interaction terms between the phases increase with calculation time caused by an oscillating solution, try using a smaler time step or a relaxation factor for the interaction terms.

I hope that helps you

Best regards

Sebastian

[mscanlon74]

Sebastian,

I actually had a breakthrough on this yesterday after doing a web meeting with one of the tech supports at Ansys. The biggest things on the set-up that he recommended changing were:

1. Switching the liquid to the continuous phase and the vapor to the dispersed phase (a different tech support at Ansys previously suggested I set it up the opposite way)

2. Not using the Wall Boiling method, he said that is really only suited for pressurized water/steam. Or the default values have really only been experimentally determined for water/steam.

Before I had the web meeting, I also took a step back and ran the flow analysis without any phase change to get some better estimates for the boundary conditions. With the results from that run, I changed the inlet and outlet to opening type B.C. instead of an actual inlet and outlet.

With these changes in the set-up it made a drastic difference. The volume fractions (at the outlet) almost completely flipped at the 10th iteration. The temperatures for the two phases at the outlet I was monitoring, both spiked at that iteration too.

For the materials, I originally started out with the Peng-Robinson type, the I switched to using them from the Interphase Mass Transfer group. The timesteps I ran the steady state simulation were 0.03 s and I didn't do anything with the relaxation factor, I've never tried that option before.

Thanks for the feedback, and hopefully passing along what I learned yesterday helps you or anyone else that may read through this.

Matt

[hamart]

Hi Dude. please help me on that if you found any solution for it. i really need it