[mkraposhin]

Dear friends!

I made model for compressible, two-phase flow with phase change due to temperature and/or pressure variation, which is based on interFoam (VOF). If you are intersted in using it, you can download it by this link (with tutorials). Solver was done for OF-2.1.0 and 1.6-ext

Equations description located here

I need your advices and feed back. I would like to put this solver in OpenFOAM - but this can take some time.

And, of course, excuse me my "great" russian english

Some nice pictures:

[Coral.Qing]

thx, i will try it if i can figure out it

[sfigato]

Hi Matvey,

thanks for share your solver!
I have some questions:

1) have you implemented the Singhal model ?? In your opinion is it difficult to do it!?
2) Can I use the solver without the hydrostatic part of the pressure (rho * g *h)?

Thanks
Regards

Marco

[zhengzh5]

Hi,

when I tried to run the steam-jet tutorial, it complains about not having the nuSgsUSpaldingWallFunction, and I couldn't find such wall function anywhere in my OpenFOAM source either, can someone point to me where to get a copy of it? if it's out there at all. thanks!

[mkraposhin]

Originally Posted by sfigato

Hi Matvey,

thanks for share your solver!
I have some questions:

1) have you implemented the Singhal model ?? In your opinion is it difficult to do it!?
2) Can I use the solver without the hydrostatic part of the pressure (rho * g *h)?

Thanks
Regards

Marco

1) Yes, but it is not included in the current release of the solver. If you will share paper with your description of this model, i can do this
2) Yes, just set g = (0 0 0)

[mkraposhin]

Originally Posted by zhengzh5

Hi,

when I tried to run the steam-jet tutorial, it complains about not having the nuSgsUSpaldingWallFunction, and I couldn't find such wall function anywhere in my OpenFOAM source either, can someone point to me where to get a copy of it? if it's out there at all. thanks!

This problem shows that you are using incorrect version OpenFOAM. Current version of OpenFOAM - 2.1.0

[mkraposhin]

Originally Posted by mkraposhin

Dear friends!

I made model for compressible, two-phase flow with phase change due to temperature and/or pressure variation, which is based on interFoam (VOF). If you are intersted in using it, you can download it by this link (with tutorials). Solver was done for OF-2.1.0 and 1.6-ext

Equations description located here

I need your advices and feed back. I would like to put this solver in OpenFOAM - but this can take some time.

And, of course, excuse me my "great" russian english

Some nice pictures:

Dear friends,

Solver code has been changed. Also, system of equations changed too.
Latest description of the test cases and description you can find here!

Today this solver works well with two type of problem:
1) Cavitation (water)
2) Flashing of water in the adiabatic conditions

Again, solver is available only for OpenFOAM 2.1.0, but i hope to port it to OF2.2.X, OF1.6-ext

[sfigato]

Originally Posted by mkraposhin

1) Yes, but it is not included in the current release of the solver. If you will share paper with your description of this model, i can do this
2) Yes, just set g = (0 0 0)

Hi,

here is the link, where you can download the description of the model:

http://fluidsengineering.asmedigital...icleid=1429576

The model includes also the gas cavitation! You cannot find the full description of the model with the gas mass transfer (one more transport equation)! If you give to me your mail I will send to you it!

thank you for sharing your work
Best Regards

Marco

[mkraposhin]

Originally Posted by sfigato

Hi,

If you give to me your mail I will send to you it!

Marco

I sent my e-mail address to you by using private message

[mkraposhin]

Originally Posted by sfigato

The model includes also the gas cavitation!

Marco

I think, it can be a problem. If gas volume fraction is small enough, and it's density is comparable to density of vapour, then we can neglect influence of the gas on the flow. So we can decouple gas fraction transport from the liquid/vapour transport.

But, if the gas volume fraction is large, then we need a coupled solution, and this can be a slightly more complex case

[mkraposhin]

Originally Posted by sfigato

1) have you implemented the Singhal model ?? In your opinion is it difficult to do it!?

Done with the source code and paper, which you sent to me by e-mail.
Source code and short description located here

But now i have 2 questions:
1) Dimensions of equation (15) are different from (13). Does it mean that constant Ce should have dimensions [meter/second]?
[(eq.13)]=kg/(meter^3 secod)

2) In equations (15) and (16) we can see mass fractions (Fv and Fl), but in our model we are solving for volume fraction. Why did you commented corresponding terms rho2/rho and rho1/rho ?

[sfigato]

Originally Posted by mkraposhin

Done with the source code and paper, which you sent to me by e-mail.
Source code and short description located here

But now i have 2 questions:
1) Dimensions of equation (15) are different from (13). Does it mean that constant Ce should have dimensions [meter/second]?
[(eq.13)]=kg/(meter^3 secod)

2) In equations (15) and (16) we can see mass fractions (Fv and Fl), but in our model we are solving for volume fraction. Why did you commented corresponding terms rho2/rho and rho1/rho ?

Great! First of all! I already validate the Singhal mass transfer model , so we can trust about the implementation!

Answer 1) The dimension of the constants actually is [meters/seconds]. This is due to an author's trick!

Answer 2) To implement the Singhal model I follwed the Tobias Huuva Thesis (this thesis is too long to send but I will send tomorrow just the Sighal Model page)! He replaces the mass fraction with the vapour one. The reason is that the transport equations of Singhal are written for the mass fractions so Singhal needs to scale the vapour fractions! The transport equations in OpenFoam are already written for the vapour fracions so you do not need to scale them!

Fhurter improvements:

1) I have already implemented th Zwart model

link: http://www.google.de/url?sa=t&rct=j&...50310824,d.Yms

It is the Ansys cavitation model and I already validated this implementation..if you want I can send to you tomorrow!

2) What is a real improvement (which no-one has already done) is to take in account for the Gas Cavitation (from equation 24 to equation 30 in Sighal's lecture )! It becomes very important in the past few years (for example for mineral oil applications)! But your model needs to be 4 phases (with condensable and non condesable gas vapour and liquid) and you must add two new transport eqautions. If you want to implement it I can share to you my knowledge (the Singhal model is not clear deriveted and I already made some new impromvents in the mass transfer rates)!

Let me know (by mail too for the two improvments)

regards
Marco

[mkraposhin]

Originally Posted by sfigato

Answer 2) To implement the Singhal model I follwed the Tobias Huuva Thesis (this thesis is too long to send but I will send tomorrow just the Sighal Model page)! He replaces the mass fraction with the vapour one. The reason is that the transport equations of Singhal are written for the mass fractions so Singhal needs to scale the vapour fractions! The transport equations in OpenFoam are already written for the vapour fracions so you do not need to scale them!

Maybe i'm stupid, but here i can't agree with you, because:
1) Av*rhov=rhom*Fv (Av - vapour volume fraction, rhov - vapor density, rhom - mixture density, Fv - mass vapour fraction)
then
ddt(Fv*rhom)+div(Fv*rhom*U)=ddt(Av*rhov) + div(Av*rhov*U)

so, OpenFOAM formulation for Av transport is the same as in Singhal paper

2) Fv in eq, (15) comes from eq. (13) where Av*rhov/rhom=Fv, isn't it?

Please, tell me where am i wrong?

[mkraposhin]

Originally Posted by sfigato

1) I have already implemented th Zwart model

link: http://www.google.de/url?sa=t&rct=j&...50310824,d.Yms

Marco

I added this model to the solver too, and now i'm running test case for hemispherical body. first results will be available tomorrow, or maybe next day after tomorrow.

Also, can you propose your test cases for this models?

[sfigato]

Originally Posted by mkraposhin

I added this model to the solver too, and now i'm running test case for hemispherical body. first results will be available tomorrow, or maybe next day after tomorrow.

Also, can you propose your test cases for this models?

Hi,

I already sent to you an mail!

Regarding the test case, I have also an hydraulic resistence with mineral oil. Moreover, I am preparing an hydraulic valve with cavitation (the geometry looks like really cool).. but it takes time to be ready!

Regards
Marco

[mkraposhin]

Hi, i made update to the solver it is available at the same address

Test cases for the hemispherical body with the Zwart and the Singhal models are still running.

Some notes on the implementation of volume fraction transport in OpenFOAM.
1)
It is formulated in volume fluxes, but it derived from mass fluxes:
ddt(alpha_l * rho_l) + div(alpha_l * rho_l * U) = m_l

ddt(alpha_l) + div(alpha_l U_l) = m_l/rho_l + (alpha_l/rho_l)*DDt(rho_l)

when fluid is incompressible and flow is isothermal, last term is zero, then we have:
ddt(alpha_l) + div(alpha_l U_l) = m_l

m_l - is the sum of m^+ and m^- of the Singhal model. In OpenFOAM m_l is represented by method mDotAlphal. That's why i think that we need to scale terms in Singhal model when switching from the mass fraction to the volume fraction

2)
In Singhal model pressure difference is calculated as: dP=pSat + c*k - p, but OpenFOAM interPhaseChangeFoam solver do not contain term "c*k" in the equation for pressure. And there is no such term in my model. That's why i don't include 0.5*0.39*rho_l*k when i estimate mass evaporation term.
If you want to insert this term in the model (interPhaseChangeFoam or compressibleMixingPhaseChangeFoam), then you need to change equation for pressure to obtain mass and momentum continuity

About NCG.
I think, i can add transport equations for the non-condensible gas in the model in three step:
1) Simple transport of the volume gas fraction without accounting for it's influence on the total mass of the system (alpha_g <= 1.0e-5 or another small value)
2) Transport of the volume gas fraction without desorption or absorption
3) And if two previous models will work, i can try to implement model with desorption and absorption

If you are still interested, it will be nice to run test cases, which you had proposed by e-mail

[sfigato]

Hi Matvej,

1) I will try to validate the model without scaling as well! The point is that it is not clear how Singhal has derivated it. I mean, where exactly he intoduces this scaling.

2) I totally agree with you. I choose to change the all mass transfer models with the 'k' term (as well as for the pressure equation) . Because I think that turbulence effects on cavitation too!

About NCG.
I think that your three steps are right. Just some considerations:

1) You must account for other two phases (dissolved and undissolved) so the transport equations which you were speaking about (in your second point) are two. This is because there is a big diference between vapor and gas. "Dissolved vapor" is the liquid. Dissolved gas has the same property of the liquid but it is not he liquid. You must take in account its fraction in the multiphase..also because it is the limit of the fraction of released undissolved gas !

2) The absorpiton and desorption rates of Singhal show not a very good agreement with experiment. We are developing our own rates. If you are intrested I can (will) provide to you these two OpenFoam files as I did for Singhal (the same framework of the vapour cavitation)

3) I will send to you a presentation about the implementation of NCG in Ansys.

Finally, I understood that you want to upload your solver in OpenFoam. A very good test case could be the valve which I spoke about. The geomety is not easy but it presents (experimentally) both gas and water cavitation. So it could be cool to have this test case. I will manage to do it when your solver is ready. During this time I try to get familiar with your implementation and I prepare the mesh.


I am so sorry that I wrote to much! Anyway, your work is great

Regards
Marco

[ma-tri-x]

Hi Matvej

I would really like to use your solver, but I only have the versions 2.1.1, 2.2.0 and 2.2.1 on my computer. The others seem to be not available anymore as ubuntu deb packs from the openfoam site. Is there any chance to use it?
For 2.1.1 I get the message:
--> FOAM FATAL IO ERROR:
[0] keyword div(phi,psiphase1) is undefined in dictionary "/home/mkoch/Master-Arbeit/0010vers211-phasechangeFoam_try/processor0/../system/fvSchemes::divSchemes"

thanks!

[ma-tri-x]

Ah sorry, it works now. I just used my old Dictionaries which were not suitable.

Another Question: what is beta for simpleLiquid?
is it the del rho/del T in the EOS?

[mkraposhin]

Originally Posted by ma-tri-x

Ah sorry, it works now. I just used my old Dictionaries which were not suitable.

Another Question: what is beta for simpleLiquid?
is it the del rho/del T in the EOS?

Hello, ma-tri-x!

I'm sorry for the late response!

Today i'm working on the new version of this solver. The system of equations has been rewritten totally, so, please, wait about 2-4 weeks.
Of course, i will made versions for OF2.1.X and OF2.2.X

Changes are very significant,