# Cavitating model in OF

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 May 26, 2009, 22:30 Cavitating model in OF #1 New Member   w.g. zhao Join Date: Apr 2009 Posts: 6 Rep Power: 9 Hello,everyone I am studying the cavitating code, does anyone knows the cavitating model in foam?

 May 28, 2009, 10:31 #2 New Member   Anne Gosset Join Date: May 2009 Posts: 3 Rep Power: 9 Hi all, Same question here: is it based on the model by Kubota/Singhal as in Fluent or CFD Ace? Thanks for your help.

 May 28, 2009, 11:50 #3 Member   David P. Schmidt Join Date: Mar 2009 Posts: 71 Rep Power: 9 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.

 May 29, 2009, 03:20 #4 New Member   w.g. zhao Join Date: Apr 2009 Posts: 6 Rep Power: 9 Thanks Mr Schmitt; Cavitation model in Fluent is Singhal's model based on Mixture model; In OF, was your theroy used?

 May 29, 2009, 04:45 #5 New Member   Anne Gosset Join Date: May 2009 Posts: 3 Rep Power: 9 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.

 May 29, 2009, 08:13 #6 New Member   w.g. zhao Join Date: Apr 2009 Posts: 6 Rep Power: 9 Same to me

May 29, 2009, 10:00
#7
Member

David P. Schmidt
Join Date: Mar 2009
Posts: 71
Rep Power: 9
Quote:
 Originally Posted by zhaowg 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

 April 16, 2010, 02:47 #8 Senior Member   Mohammad Join Date: Feb 2010 Location: Shiraz, Iran Posts: 108 Rep Power: 8 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.

 May 3, 2010, 17:12 #9 Member     Marta Lazzarin Join Date: Jun 2009 Location: Italy Posts: 70 Rep Power: 9 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

 May 6, 2010, 03:39 There are actually two cavitation models in OF #10 New Member   Oscar Join Date: Jun 2009 Location: Murcia, Spain Posts: 14 Rep Power: 9 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.

 May 6, 2010, 06:15 #11 Member     Marta Lazzarin Join Date: Jun 2009 Location: Italy Posts: 70 Rep Power: 9 Ok, i'll have a try with the other solver and see. Thank you very much for your quick reply = ) ! Marta

 May 6, 2010, 07:25 #12 New Member   w.g. zhao Join Date: Apr 2009 Posts: 6 Rep Power: 9 yea, 1.6.x have an example in the tutorial.

 January 17, 2012, 05:17 #13 New Member   Majid S. Join Date: Jan 2012 Location: mumbai Posts: 11 Rep Power: 6 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.

 January 17, 2012, 10:37 courant number #14 New Member   saeed rakhsha Join Date: Jan 2012 Location: iran-tehran Posts: 1 Rep Power: 0 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.

 March 3, 2012, 11:43 Merkle model and cavitation #15 Senior Member   ehsan Join Date: Mar 2009 Posts: 106 Rep Power: 9 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

 June 6, 2012, 23:47 kin-energy-turb #16 Member   vahid Join Date: Feb 2012 Location: Mashhad-Iran Posts: 80 Rep Power: 5 Hello dear foames, I have an easy question, i wanna add the kinetic Turbulence energy (k) in model <> for solver <>. 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: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

 July 14, 2013, 19:08 #17 New Member   erfan-BA Join Date: Jun 2013 Posts: 4 Rep Power: 5 hi, i want to simulate cavitation in gear pump with foam.can you help me to solve my problem? kind regArds, behnam.

December 25, 2014, 02:37
#18
New Member

BO
Join Date: Dec 2014
Posts: 21
Rep Power: 4
Quote:
 Originally Posted by schmidt_d 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. : )

 December 25, 2014, 16:57 Cavitation in Fluent #19 New Member   samir Join Date: Sep 2011 Location: Algeria Posts: 11 Rep Power: 7 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

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

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

All times are GMT -4. The time now is 00:20.

 Contact Us - CFD Online - Top