[Reza_CFD]

Hello friends,
I would like to simulate pool boiling in a box, using interPhaseChangeFoam. I am using OpenFOAM 2.3.
However, I cannot see any change in alpha.water, although the temperature of the walls are higher than saturated temperature.
Is anybody here to help me?

Thanks,
Reza

[Reza_CFD]

That's very weird since the temperature field covers a broad range of temperature, including below and above the saturation temperature. However, I don't see any change in alpha.water as such it remains one.
Have you ever encountered this issue?

Thanks

[Reza_CFD]

I think I got the reason, however I cannot solve the issue.
In fact, I am modifying the interPhaseChangeFoam based on the work by Andersen at http://www.tfd.chalmers.se/~hani/kur...ChangeFoam.pdf

When I add the temperature equation, I cannot see change in volume fractions of water.
Is there any comment, help?

Thanks

[Reza_CFD]

Seems nobody is interested.

[Reza_CFD]

The problem in this work is that I get negative temperature.
Do you have any clue to resolve this problem?

Thanks

[Parisa_Khiabani]

Hey Reza,
Did you solve your problem? Please let me know since I think my case is very similar to yours.

Thanks,
Parisa

-----

I am aware that there have been lots of discussions about bugs in interPhaseChangeFoam in 2.1.0 and then the bug was resolved in 2.1.x.
However, I am following the tutorial by Martin Andersen and I added the energy equation as well as temperature dependent PSat.
But, I got completely unrealistic results. PSat become zero in many places in the domain since the temperature dropped much below zero.
Is there any solution for that?

Thanks,
Parisa

[Parisa_Khiabani]

Please let me clarify myself.
The energy equation is solved without any problem, and actually I obtained reasonable temperature distribution.
However, as soon as the temperature dependent PSat is inserted, the solver becomes confused and generate some unrealistic results.
So, I think the problem is coupling between PSat and temperature distribution.
I appreciate if you help me at this.

Thanks,
Parisa

[Parisa_Khiabani]

I also have the same problem with OpenFOAM 2.2.x.

Any help?

[Parisa_Khiabani]

Just more updates on my problem.
I am solving the same case in OpenFOAM 2.3. In fact there is no phase change inside the domain.
I am looking forward to hearing from you guys,

Thanks,
Parisa

[Parisa_Khiabani]

Please, I am really anticipating any kind of help.

Parisa

[wyldckat]

Greetings to all!

I've merged your two threads into a single one, since almost the exact same problem. This way it makes it easier for other people to find this thread to help or to find help in any answers that can arise.

Regarding your questions, I've taken a quick look at the PDF by Andersen, that Reza pointed out, and the first detail that popped up to me was: the original author used OpenFOAM 2.0.x.

Now, you might not be familiar with how OpenFOAM evolves over time, but from personal experience I can tell you that solvers can change considerably between versions of OpenFOAM, therefore the probabilities of making an example that works on 2.0.x, work on 2.1.x or 2.3.x, requires some considerable time and experience.

Therefore, the first step you should take is to install OpenFOAM 2.0.x and then test the case with that version.

Secondly, it takes quite some time to set-up an example case that you're working on, therefore it makes it a lot harder for someone with more experience to step in and spend 2-5h trying to reproduce the same steps. Therefore, please read, study and follow these instructions: http://www.cfd-online.com/Forums/ope...-get-help.html

Best regards,
Bruno

[Reza_CFD]

First of all thanks from wyldckat for the nice and professional explanation.
Parisa:

I am sorry for delay in response. I solved that issue. However, I am changing the solver and I am using interFoam. I updated the solver with mass transfer and temperature distribution. I hesitate sending the code to you since it's not complete yet.
Maybe the experts can help me, then I will resolve the problem and make the code ready for you.
The problem is that the code is running for some time steps, I get boiling, and/or condensation. The results are convincing and somehow I validated with some solid results.
However, after a while, the courant number increases rapidly and the rsults are ruined such that the volume fractions reach to -50 and +600.
I use very low deltaT, and also adjustdeltaT is on.
Any help, comment. suggestion from experts?

Thanks everybody for the nice cooperation.
Reza

Originally Posted by wyldckat

Greetings to all!

I've merged your two threads into a single one, since almost the exact same problem. This way it makes it easier for other people to find this thread to help or to find help in any answers that can arise.

Regarding your questions, I've taken a quick look at the PDF by Andersen, that Reza pointed out, and the first detail that popped up to me was: the original author used OpenFOAM 2.0.x.

Now, you might not be familiar with how OpenFOAM evolves over time, but from personal experience I can tell you that solvers can change considerably between versions of OpenFOAM, therefore the probabilities of making an example that works on 2.0.x, work on 2.1.x or 2.3.x, requires some considerable time and experience.

Therefore, the first step you should take is to install OpenFOAM 2.0.x and then test the case with that version.

Secondly, it takes quite some time to set-up an example case that you're working on, therefore it makes it a lot harder for someone with more experience to step in and spend 2-5h trying to reproduce the same steps. Therefore, please read, study and follow these instructions: http://www.cfd-online.com/Forums/ope...-get-help.html

Best regards,
Bruno

[wyldckat]

Hi Reza,

Originally Posted by Reza_CFD

The problem is that the code is running for some time steps, I get boiling, and/or condensation. The results are convincing and somehow I validated with some solid results.
However, after a while, the courant number increases rapidly and the rsults are ruined such that the volume fractions reach to -50 and +600.
I use very low deltaT, and also adjustdeltaT is on.
Any help, comment. suggestion from experts?

Mmm... OK, not much information to work with. There are several possibilities that come to my mind:

1. The mesh is to blame, because it has either very big, very small or bad looking cells. Have a look at this blog post of mine, to better understand what I'm referring to: OpenFOAM: Interesting cases of bad meshes and bad initial conditions - more specifically, "Case two", which is the one conceptually more similar.
2. Still from the previous link and case, you'll notice how I diagnosed the problem. More specifically, instead of being only interested in the solution and writing only occasional time snapshots, I configured it to write as many time steps as possible, so that I could carefully examine how the flow behaved in certain locations.
3. When dealing with evaporation, it's easy to enter the compressible working range. Perhaps you should use compressibleInterFoam instead.
4. I'm also guessing here, but probably you're reaching temperatures or pressure differences that are not contemplated by the simulation model you're using.
5. Running in parallel can sometimes give unexpected results. When developing a new solver, you should always only run in serial, until you are able to have a properly working and tested solver. Then run in parallel the same validated case, to diagnose if it still gives you the same results.

Best regards,
Bruno

[Kanarya]

Hi Reza,

I am interested in condensation and do you think interFoam is more suitable to solve the problem in comparison to interPhaseChangeFoam?
Did you managed to solve the problem?
Thanks in advance!
best regards,

Originally Posted by Reza_CFD

First of all thanks from wyldckat for the nice and professional explanation.
Parisa:

I am sorry for delay in response. I solved that issue. However, I am changing the solver and I am using interFoam. I updated the solver with mass transfer and temperature distribution. I hesitate sending the code to you since it's not complete yet.
Maybe the experts can help me, then I will resolve the problem and make the code ready for you.
The problem is that the code is running for some time steps, I get boiling, and/or condensation. The results are convincing and somehow I validated with some solid results.
However, after a while, the courant number increases rapidly and the rsults are ruined such that the volume fractions reach to -50 and +600.
I use very low deltaT, and also adjustdeltaT is on.
Any help, comment. suggestion from experts?

Thanks everybody for the nice cooperation.
Reza

[mihaipruna]

there is one extra step for Martin Andersen's tutorial that is not specified I believe:

you have to recompile the phaseChangeTwoPhaseMixture, by going in that folder and typing wclean and then wmake.
Make sure you first go in the file called files in the make folder in phaseChangeTwoPhaseMixture and change to LIB= $(FOAM_USER_LIBBIN) etc instead of $(FOAM_LIBBIN)

then (dunno if you need to do that) do wmake from the myInterPhaseChangeFoam folder

This at least makes the alpha change, not sure about the results

[Kanarya]

thanks for the answer!

did you implement is to latest version of OF or 210?

Originally Posted by mihaipruna

there is one extra step for Martin Andersen's tutorial that is not specified I believe:

you have to recompile the phaseChangeTwoPhaseMixture, by going in that folder and typing wclean and then wmake.
Make sure you first go in the file called files in the make folder in phaseChangeTwoPhaseMixture and change to LIB= $(FOAM_USER_LIBBIN) etc instead of $(FOAM_LIBBIN)

then (dunno if you need to do that) do wmake from the myInterPhaseChangeFoam folder

This at least makes the alpha change, not sure about the results

[mihaipruna]

Version 2.3.1
The tutorial should be applied pretty much the same way except for the extra compilation for the libraries i mentioned

Also there is a Tfinal field in fvSolution which I made the same as T, not sure what it does yet

You don't have to do this part: #include "../interFoam/correctPhi.H"

I am still having issues with Courant number blowing up

[mihaipruna]

I think I have figure out how to get decent behavior, with decent time step size that allows you to simulate over longer periods of time.

I believe the evaporation rate was unphysical.
I used the Kunz model into the transport properties and looked deeper into how the coefficients are determined:
dimensionedScalar UInf_;
dimensionedScalar tInf_;
dimensionedScalar Cc_;
dimensionedScalar Cv_;

Uinf is the reference velocity, I set it to something like 1m/s.
tinf I set dividing the diameter of the vessel by Uinf.

Cc_ and Cv_ are proportional to the phase change rate.In a nutshell, the smaller they are, the smaller the evaporation rate, which would in turn lowers the maximum Courant number it gets to.
In this paper: http://www.personal.psu.edu/faculty/...MEsummer99.pdf they were set to 0.2, which are values determined experimentally.
Of course, you might have to set different numbers, especially since you are not doing cavitation, but rather, boiling.

What I plan to do next is correlate the volume fraction/time obtained from CFD with a simple system analysis spreadsheet I did for my vessel, where I can vary some parameters and observe the boiling through basic formulas independent of geometry save for general sizing.

Then I will change the Cc_ and Cv_ values accordingly to match the same evaporation rate on gross terms.

[Kanarya]

Hi,
I am not getting the correct results from when I set the inlet BC for alpha =0 which is vapur...I do not see any condensation in side the tube..what kind of geometry are you using? I am trying t simulate pipe flw but I am not sure about alpha and p_rgh BC?
do you have any idea?

Thanks in advance!

Originally Posted by mihaipruna

I think I have figure out how to get decent behavior, with decent time step size that allows you to simulate over longer periods of time.

I believe the evaporation rate was unphysical.
I used the Kunz model into the transport properties and looked deeper into how the coefficients are determined:
dimensionedScalar UInf_;
dimensionedScalar tInf_;
dimensionedScalar Cc_;
dimensionedScalar Cv_;

Uinf is the reference velocity, I set it to something like 1m/s.
tinf I set dividing the diameter of the vessel by Uinf.

Cc_ and Cv_ are proportional to the phase change rate.In a nutshell, the smaller they are, the smaller the evaporation rate, which would in turn lowers the maximum Courant number it gets to.
In this paper: http://www.personal.psu.edu/faculty/...MEsummer99.pdf they were set to 0.2, which are values determined experimentally.
Of course, you might have to set different numbers, especially since you are not doing cavitation, but rather, boiling.

What I plan to do next is correlate the volume fraction/time obtained from CFD with a simple system analysis spreadsheet I did for my vessel, where I can vary some parameters and observe the boiling through basic formulas independent of geometry save for general sizing.

Then I will change the Cc_ and Cv_ values accordingly to match the same evaporation rate on gross terms.

[mihaipruna]

As I posted earlier in the thread, to get it to work for me, I had to recompile
phaseChangeTwoPhaseMixture