CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM

Cavitating model in OF

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree3Likes
  • 3 Post By schmidt_d

Reply
 
LinkBack Thread Tools Display Modes
Old   May 26, 2009, 22:30
Default Cavitating model in OF
  #1
New Member
 
w.g. zhao
Join Date: Apr 2009
Posts: 6
Rep Power: 8
zhaowg is on a distinguished road
Hello,everyone
I am studying the cavitating code, does anyone knows the cavitating model in foam?
zhaowg is offline   Reply With Quote

Old   May 28, 2009, 10:31
Default
  #2
New Member
 
Anne Gosset
Join Date: May 2009
Posts: 3
Rep Power: 8
Anneg is on a distinguished road
Hi all,

Same question here: is it based on the model by Kubota/Singhal as in Fluent or CFD Ace?

Thanks for your help.
Anneg is offline   Reply With Quote

Old   May 28, 2009, 11:50
Default
  #3
Member
 
David P. Schmidt
Join Date: Mar 2009
Posts: 70
Rep Power: 8
schmidt_d is on a distinguished road
Hi,

No, the Kubota model is quite different from what is in OpenFOAM. The Kubota model is a Rayleigh-Plesset based model, where you model bubble growth or collapse. OpenFOAM's cavitation models belong to a class of Homogenous Equilibrium Models. The details of the implementation change from solver to solver and with sequential releases of OF.

The basic idea is that the liquid and vapor are homogenously mixed within a cell (no interface tracking), which is appropriate for very high Weber numbers where the interface is so convoluted, VOF reconstruction would be pointless. Because of the large surface area and the large liquid-to-vapor density ratio, there is also no reason to solve a separate momentum equation for the vapor, which is transporting a trivial amount of momentum. Finally, we assume that the two-phases are in thermodynamic equilibrium, with inertia limiting phase change and heat transfer being relatively fast. This last assumption is only valid for certain cavitating regimes, with low temperatures and small length scales.

If you make these assumptions, you can work up a rule for the compressibility of the mixture. This closes the problem, though numerically, handling the very rapid changes in compressibility takes some care.

I used this HEM approach successfully for modeling cavitation in diesel fuel injectors. I have been very happy with it. My implementation, numerically, was built like a high-Mach number solver. It was simple, but very efficient for the kinds of high velocities, 400 m/s, you see in modern diesel injector nozzles. I give out the F77 code for those curious, hardy souls. For low speed flows, you would never want to construct your code the way that I made mine.

The OpenFOAM'ers have generalized the numerical approach to permit calculations more efficiently at lower velocities. That is great and of course you get all the beautiful flexibility of OF: parallelism, polyhedral meshes. The downside is that OF is collocated, which makes pressure/velocity coupling more difficult. As a consequence, you may run into stability problems and noise. I'd be interested in seeing papers from people who have applied the OF cavitation codes.

I also have some papers to share; I've written a bit about HEM modeling of cavitation, including a new paper to appear next month at ICLASS that explores the assumption of thermodynamic equilibrium. I'd be happy to send that out.

-David Schmidt
zandi, nipinl and 88481101 like this.
schmidt_d is offline   Reply With Quote

Old   May 29, 2009, 03:20
Default
  #4
New Member
 
w.g. zhao
Join Date: Apr 2009
Posts: 6
Rep Power: 8
zhaowg is on a distinguished road
Thanks Mr Schmitt;
Cavitation model in Fluent is Singhal's model based on Mixture model;
In OF, was your theroy used?
zhaowg is offline   Reply With Quote

Old   May 29, 2009, 04:45
Default
  #5
New Member
 
Anne Gosset
Join Date: May 2009
Posts: 3
Rep Power: 8
Anneg is on a distinguished road
Thanks for the explanations.
My intention is to test this cavitation model in OF on hydrofoils and propellers in the close future. Hopefully, papers will follow.
Anneg is offline   Reply With Quote

Old   May 29, 2009, 08:13
Default
  #6
New Member
 
w.g. zhao
Join Date: Apr 2009
Posts: 6
Rep Power: 8
zhaowg is on a distinguished road
Same to me
zhaowg is offline   Reply With Quote

Old   May 29, 2009, 10:00
Default
  #7
Member
 
David P. Schmidt
Join Date: Mar 2009
Posts: 70
Rep Power: 8
schmidt_d is on a distinguished road
Quote:
Originally Posted by zhaowg View Post
Thanks Mr Schmitt;
Cavitation model in Fluent is Singhal's model based on Mixture model;
In OF, was your theroy used?
Similar physics, very different numerics. I'm pretty confident about the applicability of physics to small, high-speed nozzles, and not so confident about the applicability to hydrofoils/props. Some modelers from Singapor published papers (JCP? Computers & Fluids? ) where they modified my model and applied it to large-scale underwater explosions. That was a surprise.

-David
schmidt_d is offline   Reply With Quote

Old   April 16, 2010, 02:47
Default
  #8
Senior Member
 
Mohammad
Join Date: Feb 2010
Location: Shiraz, Iran
Posts: 108
Rep Power: 7
m2montazari is on a distinguished road
hi,
I want to model the cavitation bubbles and more specifically the collapse of bubbles. as fluent uses mixture model for cavitation, we have no bubbles but just a region with continues change in phases and no boundaries. so the collapse cant be model in this matter.
I dont know if openfoam can help me; for example maybe the interphasechangefoam can help, but I dont know the equations it uses.
I think the famous Reighly-plesset equation can be more helpful than the model in fluent,for example.
if anyone can help, I'll be so thankful .

Mohammad.
m2montazari is offline   Reply With Quote

Old   May 3, 2010, 17:12
Default
  #9
Member
 
Marta's Avatar
 
Marta Lazzarin
Join Date: Jun 2009
Location: Italy
Posts: 69
Rep Power: 8
Marta is on a distinguished road
Hi!
We are also trying to apply the cavitatingFoam solver to analyse the behaviour of small injector holes used for N2O in hybrid rockets.

At the moment we are just verifying its stability and flexibility for this kind of problems, then we would like to compare our results with an experiment we are creating...

If anyone has tried it with this kind of applications I would be glad to exchange some information about it!

As concerns interPhaseChangeFoam, as far as I know it doesn't include the Plesset modelling of bubble growth.

Marta
Marta is offline   Reply With Quote

Old   May 6, 2010, 03:39
Default There are actually two cavitation models in OF
  #10
New Member
 
Oscar
Join Date: Jun 2009
Location: Murcia, Spain
Posts: 14
Rep Power: 8
Zowie is on a distinguished road
Well, I have been doing some simulations of cavitation in a nozzle with cavitatingFoam (RAS) and interPhaseChangeFoam (Schnerr Model, only available in OF1.6.x). Works quite good until now.
Zowie is offline   Reply With Quote

Old   May 6, 2010, 06:15
Default
  #11
Member
 
Marta's Avatar
 
Marta Lazzarin
Join Date: Jun 2009
Location: Italy
Posts: 69
Rep Power: 8
Marta is on a distinguished road
Ok, i'll have a try with the other solver and see.

Thank you very much for your quick reply = ) !

Marta
Marta is offline   Reply With Quote

Old   May 6, 2010, 07:25
Default
  #12
New Member
 
w.g. zhao
Join Date: Apr 2009
Posts: 6
Rep Power: 8
zhaowg is on a distinguished road
yea, 1.6.x have an example in the tutorial.
zhaowg is offline   Reply With Quote

Old   January 17, 2012, 05:17
Default
  #13
New Member
 
Majid S.
Join Date: Jan 2012
Location: mumbai
Posts: 11
Rep Power: 5
majid_esi is on a distinguished road
about ACE+ cavitation model... It uses the full cavitation model by Singhal and Athavale ...

It allows multi-dimensional simulations of cavitating flows with phase changes in low pressure regions. The model accounts for important effects such as bubble dynamics, turbulence, and the presence and expansion of non-condensable gases in liquid.
majid_esi is offline   Reply With Quote

Old   January 17, 2012, 10:37
Default courant number
  #14
New Member
 
saeed rakhsha
Join Date: Jan 2012
Location: iran-tehran
Posts: 1
Rep Power: 0
saeedrakhsha is on a distinguished road
hi
i do on the cavitation modelling in OF by interPhaseChangeFoam
the geometry is hydrofoil with rectangular domain
i don't know which courant number is appropriate for this processing,

beforehand thanks for help.
saeedrakhsha is offline   Reply With Quote

Old   March 3, 2012, 11:43
Default Merkle model and cavitation
  #15
Member
 
ehsan
Join Date: Mar 2009
Posts: 92
Rep Power: 8
ehsan is on a distinguished road
Dear All

1- Courant No of 0.5 is fine

2- In OF, we tried Sauer model fine, but once we used Merkle model code needs a very small time step. Any comment?

Regards
ehsan is offline   Reply With Quote

Old   June 6, 2012, 23:47
Default kin-energy-turb
  #16
Member
 
vahid
Join Date: Feb 2012
Location: Mashhad-Iran
Posts: 80
Rep Power: 4
vahid.najafi is an unknown quantity at this point
Hello dear foames,
I have an easy question, i wanna add the kinetic Turbulence energy (k) in model <<Sauer>> for solver <<interPhaseChangeFoam>>. For this purpose, after adding turbulence library in the option file, for introducing k in the Sauer model, this parameter is added as the follow

// * * * * * * * * * * * * * * Member Functions * * * * * * * * * * * * * * //

Foam::tmp<Foam::volScalarField>
Foam:haseChangeTwoPhaseMixtures::SchnerrSauer::r Rb
(
const volScalarField& limitedAlpha1
) const
{
return pow
(
((k_*4*constant::mathematical:i*n_)/3)
*limitedAlpha1/(1.0 + alphaNuc() - limitedAlpha1),
1.0/3.0
);
}


when I execute wmake in terminal ,this error is appeared.

phaseChangeTwoPhaseMixtures/SchnerrSauer/SchnerrSauer.C:79: error: k_ was not declared in this scope
make: *** [Make/linux64GccDPOpt/SchnerrSauer.o] Error 1

could everyone to tell me the steps of how to add the kinetic energy in the Sauer model so that after any iteration, new updated value is entered to this model ?

Regards
vahid.najafi is offline   Reply With Quote

Old   July 14, 2013, 19:08
Default
  #17
New Member
 
erfan-BA
Join Date: Jun 2013
Posts: 4
Rep Power: 4
88481101 is on a distinguished road
hi,
i want to simulate cavitation in gear pump with foam.can you help me to solve my problem?

kind regArds,

behnam.
88481101 is offline   Reply With Quote

Old   December 25, 2014, 02:37
Default
  #18
New Member
 
BO
Join Date: Dec 2014
Posts: 19
Rep Power: 2
xianqiejiao is on a distinguished road
Quote:
Originally Posted by schmidt_d View Post
Hi,

No, the Kubota model is quite different from what is in OpenFOAM. The Kubota model is a Rayleigh-Plesset based model, where you model bubble growth or collapse. OpenFOAM's cavitation models belong to a class of Homogenous Equilibrium Models. The details of the implementation change from solver to solver and with sequential releases of OF.

The basic idea is that the liquid and vapor are homogenously mixed within a cell (no interface tracking), which is appropriate for very high Weber numbers where the interface is so convoluted, VOF reconstruction would be pointless. Because of the large surface area and the large liquid-to-vapor density ratio, there is also no reason to solve a separate momentum equation for the vapor, which is transporting a trivial amount of momentum. Finally, we assume that the two-phases are in thermodynamic equilibrium, with inertia limiting phase change and heat transfer being relatively fast. This last assumption is only valid for certain cavitating regimes, with low temperatures and small length scales.

If you make these assumptions, you can work up a rule for the compressibility of the mixture. This closes the problem, though numerically, handling the very rapid changes in compressibility takes some care.

I used this HEM approach successfully for modeling cavitation in diesel fuel injectors. I have been very happy with it. My implementation, numerically, was built like a high-Mach number solver. It was simple, but very efficient for the kinds of high velocities, 400 m/s, you see in modern diesel injector nozzles. I give out the F77 code for those curious, hardy souls. For low speed flows, you would never want to construct your code the way that I made mine.

The OpenFOAM'ers have generalized the numerical approach to permit calculations more efficiently at lower velocities. That is great and of course you get all the beautiful flexibility of OF: parallelism, polyhedral meshes. The downside is that OF is collocated, which makes pressure/velocity coupling more difficult. As a consequence, you may run into stability problems and noise. I'd be interested in seeing papers from people who have applied the OF cavitation codes.

I also have some papers to share; I've written a bit about HEM modeling of cavitation, including a new paper to appear next month at ICLASS that explores the assumption of thermodynamic equilibrium. I'd be happy to send that out.

-David Schmidt
Hi David,

I just happened to see this thread 5 years ago. I am working on the cavitatingFoam currently, and it doesn't change much since your time. I wish I could do some improvement to it. Maybe more appropriate physical model. Any suggestion on this?

Many thanks! Merry Christmas by the way. : )
xianqiejiao is offline   Reply With Quote

Old   December 25, 2014, 16:57
Default Cavitation in Fluent
  #19
New Member
 
samir
Join Date: Sep 2011
Location: Algeria
Posts: 11
Rep Power: 5
samir_cfd is on a distinguished road
Send a message via MSN to samir_cfd Send a message via Skype™ to samir_cfd
Hi everybody am trying to simulate the cavitation on Fluent and I would like to know how to adjust the vaporisation pressure, the flow velocity and the gauge pressure at the outlet for a given cavitation number
Thank you for your collaboration
Samir
samir_cfd is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
references about the fan/radiator model Mihai ARGHIR Main CFD Forum 1 January 8, 2001 16:49
references about the fan/radiator model Mihai ARGHIR FLUENT 0 December 21, 2000 04:07
references about the fan/radiator model Mihai ARGHIR Main CFD Forum 0 December 21, 2000 04:06
references about the fan/radiator model Mihai ARGHIR Main CFD Forum 1 December 17, 2000 08:01
references about the fan/radiator model Mihai ARGHIR FLUENT 0 December 17, 2000 07:40


All times are GMT -4. The time now is 16:00.