# Force calculation in multiphase simulations

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

 LinkBack Thread Tools Search this Thread Display Modes
 June 4, 2012, 09:06 #21 Senior Member   Andrea Ferrari Join Date: Dec 2010 Posts: 319 Rep Power: 15 Hi, here is a summary of what i have done: 1-i created my own library called forceMultiPhase 2- in forceMultiPhase.C 1) where devRhoReff() is calculated Code: ```else if (obr_.foundObject("transportProperties")) { const dictionary& transportProperties = obr_.lookupObject("transportProperties"); const volVectorField& U = obr_.lookupObject(UName_); // return -mu*dev(twoSymm(fvc::grad(U))); return -dev(twoSymm(fvc::grad(U)));``` 2) in calcForceMoment() Code: ```const volVectorField& U = obr_.lookupObject(UName_); const volScalarField& p = obr_.lookupObject(pName_); const volScalarField& alpha1 = obr_.lookupObject("alpha1"); const dictionary& transportProperties = obr_.lookupObject("transportProperties"); dimensionedScalar nu1(transportProperties.subDict("phase1").lookup("nu")); dimensionedScalar nu2(transportProperties.subDict("phase2").lookup("nu")); dimensionedScalar rho1(transportProperties.subDict("phase1").lookup("rho")); dimensionedScalar rho2(transportProperties.subDict("phase2").lookup("rho")); //to avoid negative values const volScalarField limitedAlpha1 ( min(max(alpha1, scalar(0)), scalar(1)) ); const fvMesh& mesh = U.mesh(); const surfaceVectorField::GeometricBoundaryField& Sfb = mesh.Sf().boundaryField(); //i changed this part a bit respect to the previous post because it is more consistent with VOF in my opinion but i think that both are not correct at the interface where alpha1 is not zero or one. Maybe you can add your comments on this. The sum of the two viscous contributions gives excatly the same results that you would get without separating the forces. tmp tdevRhoReff1 = nu1*rho1*devRhoReff(); const volSymmTensorField::GeometricBoundaryField& devRhoReffb1 = tdevRhoReff1().boundaryField(); tmp tdevRhoReff2 = nu2*rho2*devRhoReff(); const volSymmTensorField::GeometricBoundaryField& devRhoReffb2 = tdevRhoReff2().boundaryField(); scalar pRef = pRef_ forAllConstIter(labelHashSet, patchSet_, iter) { label patchi = iter.key(); vectorField Md ( mesh.C().boundaryField()[patchi] - coordSys_.origin() ); //Pressure Force vectorField pf1(Sfb[patchi]*((p.boundaryField()[patchi]-pRef)*limitedAlpha1.boundaryField()[patchi])); vectorField pf2(Sfb[patchi]*((p.boundaryField()[patchi]-pRef)*(scalar(1)-limitedAlpha1.boundaryField()[patchi]))); fm.first().first() += rho(p)*sum(pf1); fm.second().first() += rho(p)*sum(pf2); //Viscous Force vectorField vf1((Sfb[patchi]*limitedAlpha1.boundaryField()[patchi]) & devRhoReffb1[patchi]); vectorField vf2((Sfb[patchi]*(scalar(1)-limitedAlpha1.boundaryField()[patchi])) & devRhoReffb2[patchi]); fm.first().second() += sum(vf1); fm.second().second() += sum(vf2); // i eliminated the moment calculation and i replaced it with force for phase 2.``` Any comments on this will be appreciated. ps if you need the library that compiles with OF 2.1.0 just give me your e-mail best andrea piaston likes this.

 September 16, 2012, 19:05 #22 New Member   Angelo J. Chaves Join Date: Aug 2012 Location: Itajubá, Brasil. Posts: 3 Rep Power: 13 Hi Andrea, I am a new user of OF, and I`ve been working with a bubble rising usinng the VOF methods. I need to calculate the drag forces at the bubble. Do you know if your solver could help me? I am using the OF 2.1.0. Thanks.

 September 18, 2012, 03:44 #23 Senior Member   Andrea Ferrari Join Date: Dec 2010 Posts: 319 Rep Power: 15 Hi, the lib forces.C calcualtes pressure and viscous force exerted by a fluid on a solid surface. If you take a look at forces.C you will see you have to specify a patch where the force is calculated. My method is the same in case of two phases flow so i guess it is not suitable for your purposes. which solver are you using? interFoam? best andrea frantov likes this.

 September 20, 2012, 16:24 #24 New Member   Angelo J. Chaves Join Date: Aug 2012 Location: Itajubá, Brasil. Posts: 3 Rep Power: 13 Hi, I`m using interDyMfoam, to achive a better result in a sorter time. But I guess that everything that works with interFoam also works with interDyMFoam. It is a shame that the solver won`t work in my case. I have been thing that changing the Forces.C, creating a new solver/application to calculate the forces where the VOF is 0.5 or some thing like that instead of calculating it in wall should solve my problem. Do You have any idea if this is possible? If it is, how i could do that? Thanks for your attention. Angelo frantov likes this.

 September 2, 2014, 23:25 #25 Member   Francisco T Join Date: Nov 2011 Location: Melbourne, Australia Posts: 64 Blog Entries: 1 Rep Power: 13 Hello I also need to calculate the drag/lift forces on a droplet. Currently force calculation needs a "patch" which are solid boundaries. Would it be possible to some how convert an isosurface to a patch? or other way Im thinking, I may need to modify the code so for the calculation of the forces, instead of a patch, uses an isosurface as an input... let me know your thoughts.. Thanks. frantov

 September 17, 2015, 11:24 #26 New Member   Daniel Rodriguez Calvete Join Date: Mar 2012 Location: Ferrol (A Coruńa) Spain Posts: 10 Rep Power: 13 Hello, I am running cavitation cases with interPhaseChangeFoam, and the tool explaned by Andrea is very useful to me. I am trying to implement it in OF 2.3, but I have a doubt about it: I see in this code that Pressure Forces is integrated multiplying by rho(p) which is 1 if the pDimensions = Pascals according to this piece of code: Code: ``` Foam::scalar Foam::forceMultiPhase::rho(const volScalarField& p) const { if (p.dimensions() == dimPressure) { return 1.0; } else { if (rhoName_ != "rhoInf") { FatalErrorIn("forceMultiPhase::rho(const volScalarField& p)") << "Dynamic pressure is expected but kinematic is provided." << exit(FatalError); } return rhoRef_; } }``` Maybe I am missunderstanding something in the code of Andrea, but since the pressure forces is the integration of pressure through the surface, I think it has not sense to multiply by rho*alpha or rho*(1- alpha) to obtain this forces. What I propose is the next piece of code in forceMultiPhace.C in calcForcesMoment() class (notice that is for OF2.3): Code: ``` vectorField fN ( Sfb[patchI]*(p.boundaryField()[patchI] - pRef) * ); // Viscous Forces vectorField fT ( ((Sfb[patchI]*limitedAlpha1.boundaryField()[patchI]) & devRhoReffb1[patchI]) + ((Sfb[patchI]*(scalar(1)-limitedAlpha1.boundaryField()[patchI])) & devRhoReffb2[patchI]) );``` I will appreciate a lot your comments about. Thank you in advance. DRC Last edited by DanielRCalvete; September 17, 2015 at 12:49.

 September 17, 2015, 15:44 #27 Senior Member   Andrea Ferrari Join Date: Dec 2010 Posts: 319 Rep Power: 15 Hi Daniel, i made the script a long time ago and i am not using it anymore..it took me a while to figure out what i did . Anyway, as you said the multiplication with rho does not have an influence since rho(p)==1 in all interWhatEverFoam solvers. Rho was there because i adapted the script from single-phase where usually the pressure is defined as p=p/rho. So you have to multiply by rho to get the correct value/dimension of the force. The multiplication with alpha1/(1-alpha1) was there because i wanted to separate the contribution in the two phases. If you dont multiply by alpha you get the total pressure force integrated on the surface (in both phases). Hope this help Andrea

 September 18, 2015, 12:32 #28 New Member   Daniel Rodriguez Calvete Join Date: Mar 2012 Location: Ferrol (A Coruńa) Spain Posts: 10 Rep Power: 13 Thank you Andrea for your fast answer. Aha!, It is question of dimension consistency, so now it is clear to me. I will use this tool in my project, thanks. Regards, sherif35 likes this.

October 20, 2015, 18:38
#29
New Member

AI
Join Date: Jun 2014
Posts: 17
Rep Power: 11
Quote:
 Originally Posted by DanielRCalvete Thank you Andrea for your fast answer. Aha!, It is question of dimension consistency, so now it is clear to me. I will use this tool in my project, thanks. Regards,
Daniel or Andrea,

Is it possible to share the library that compiles with OF 2.3?
I'm trying to calculate forces on a cylinder in a 2 phase flow with sharp interface using LES and I'm interested in calculating the forces on the cylinder for each phase separately. Thank you very much.

Ahmed

 January 26, 2016, 04:14 #30 Member   Giovanni Caramia Join Date: Mar 2009 Location: Bari, ITALY Posts: 58 Rep Power: 16 Hello, I am using interPhaseChangeFoam OF2.3.1. I am sorry but reading the previous posts I did not understand if the force calculation over a patch, as originally done in OF2.3.1, is correct or not. Thank you!

 November 5, 2019, 07:32 #31 New Member   Nguyen Minh Quan Join Date: Feb 2019 Posts: 2 Rep Power: 0 Hi Andrea, I post this because I'm interested in calculating wave force (2 phases flow) exerted on a structure. It's seem a very classical problem and the original post was 7 years old, so I'm wondering if the functionality is already implemented in official release? Actually I'm using the libforce but the force was underestimated, and when I look into force.C there are no lookup for alpha value? My wild guest was the library is still not intended to be used for multi-phase flow (which is strange?) or I'm making some mistake by setting the rhoInf = 998.8? Could you please share me your code (thichdore@gmail.com)? Thank you in advance. Quan

 January 4, 2021, 08:13 #32 New Member   Join Date: Oct 2016 Posts: 4 Rep Power: 8 Hello everyone, It has been ages since this thread was created but it seems that the tool for analysing forces in multiphase simulations still has not been implemented. Does anyone have a custom library and would be able to share it? I can give you my email in PM. Any help would be greatly appreciated. Cheers!

January 5, 2021, 02:55
#33
Senior Member

Join Date: Dec 2019
Location: Cologne, Germany
Posts: 326
Rep Power: 7
Quote:
 Originally Posted by Adq4 Hello everyone, It has been ages since this thread was created but it seems that the tool for analysing forces in multiphase simulations still has not been implemented. Does anyone have a custom library and would be able to share it? I can give you my email in PM. Any help would be greatly appreciated. Cheers!
hi,
in fact, that is not true anymore. you can output forces for multiphase simulations.

in controlDict you need to add these lines:
from phaseForces.H in OF 7:
Example of function object specification:
\verbatim
phaseForces.water
{
type phaseForces;
libs ("libreactingEulerFoamFunctionObjects.so");
writeControl writeTime;
writeInterval 1;

...

phaseName water;
}
\endverbatim

January 5, 2021, 08:08
#34
New Member

Join Date: Oct 2016
Posts: 4
Rep Power: 8
Hi geth03,

thanks for your response. This is what I found about phaseForces in the API Guide for v2006:

Quote:
 This function object calculates and outputs the blended interfacial forces acting on a given phase, i.e. drag, virtual mass, lift, wall-lubrication and turbulent dispersion. Note that it works only in run-time processing mode and in combination with the reactingEulerFoam solvers.
However, I am dealing with air-oil simulation using interFoam and I am interested in forces acting on a specific patch - solid wall. Despite that, I attempted to implement phaseForces into my controlDict but it does not seem to be recognized at all no matter what I change...

Do you think this feature is applicable to such case?

Many thanks.

January 5, 2021, 13:15
#35
Senior Member

Join Date: Dec 2019
Location: Cologne, Germany
Posts: 326
Rep Power: 7
Quote:
 Originally Posted by Adq4 Hi geth03, thanks for your response. This is what I found about phaseForces in the API Guide for v2006: However, I am dealing with air-oil simulation using interFoam and I am interested in forces acting on a specific patch - solid wall. Despite that, I attempted to implement phaseForces into my controlDict but it does not seem to be recognized at all no matter what I change... Do you think this feature is applicable to such case? Many thanks.
No its not, bc it is implemented for phase pairs.

What exactly do you want to compute and where exactly? Do you have any equations that need to be solved? Is it enough if you write out only a single value into a txt file or do you want to output cell data to open with paraview?

If you provide more information, we could think about a smart solution .

January 7, 2021, 10:13
#36
New Member

Join Date: Oct 2016
Posts: 4
Rep Power: 8
Hi geth03,

Ideally, I would like to track a convergence of forces acting on a specific set of patches in my multi-phase simulations as one does with forces function object in single-phase cases.
One time step - one line of data into postProcessing folder:

Quote:
 # Moment # CofR : (0.000000e+00 0.000000e+00 0.000000e+00) # # Time (total_x total_y total_z) (pressure_x pressure_y pressure_z) (viscous_x viscous_y viscous_z) ... 127 (-2.1e-06 1.2e-06 2.3e-04) (-1.9e-06 3.1e-06 0.0e+00) (-2.2e-07 -1.9e-06 2.3e-04) ...
My cases are 3D and laminar and employ interFoam solver. For simplicity, we can discuss a tutorial case such as mixerVessel2D. How would you track forces acting on the rotor? I know it's possible to extract forces using ParaView but that's just too cumbersome if you have more than a single case and it doesn't allow you to follow the development at every single time step...

Any suggestions on this?

Cheers.

 January 8, 2021, 03:28 #37 Senior Member   Join Date: Dec 2019 Location: Cologne, Germany Posts: 326 Rep Power: 7 ok, first of all you need a postProcessing utility like the one you gave as an example, so basically you could look at the source code and figure out the syntax and make changes according to your needs. you can either extend it or even delete the stuff you don't need and just keep the stuff you need. either way, you should be able to reach your goal, it is not a big task. i hope you have some basic c++ programming skills.

 January 8, 2021, 04:46 #38 New Member   Join Date: Oct 2016 Posts: 4 Rep Power: 8 Hi geth03, I understand it's possible to create a custom function object for this. However, my understanding of the source code is limited and my experience with C++ is 0 as of today. I hoped that someone might be able to share with me a sample library or something similar so I wouldn't need to start from scratch. Otherwise, I'll do it myself but it'll surely take more time than I would like. Cheers.

 Thread Tools Search this Thread Search this Thread: Advanced Search 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 Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Mohammad Faridul Alam CFX 4 January 11, 2013 07:19 rjmcsherry CFX 2 October 21, 2010 10:34 JPBodner Main CFD Forum 3 August 4, 2010 11:11 Susan YU FLUENT 0 June 2, 2010 08:46 cwang5 OpenFOAM Programming & Development 1 May 4, 2010 04:59

All times are GMT -4. The time now is 17:49.

 Contact Us - CFD Online - Privacy Statement - Top