# Problems in understanding BuoyantBoussinesqSimpleFoam

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

August 24, 2011, 11:41
Problems in understanding BuoyantBoussinesqSimpleFoam
#1
Senior Member

Anne Gerdes
Join Date: Aug 2010
Location: Hamburg
Posts: 168
Rep Power: 11
Dear Foamers,

I still habe problems in understanding the source code of BuoyantBoussinesqSimpleFoam.

In the attachment you see the momentum equation which has to be solved where GT= rho g= (1-beta(T-T_0))*g

In pEqn.H the main code is settled.

First the velocity is solved without taking into account pressure or density.
HTML Code:
`U = rAU*UEqn().H();`
The flux is the interpolation of this velocity.
HTML Code:
`phi = fvc::interpolate(U) & mesh.Sf();`
Then a buoyancy flux is defined

HTML Code:
`surfaceScalarField buoyancyPhi(rAUf*ghf*fvc::snGrad(rhok)*mesh.magSf());`
Here my first question: Why is the normal gradient computed? In the equation there is only a term which includes the density, not the gradient of the density.

The flux is corrected with the buoyancy flux

HTML Code:
` phi -= buoyancyPhi;`
After the pressure correction with the Laplace equation

HTML Code:
`fvm::laplacian(rAUf, p_rgh) == fvc::div(phi)`
the flux is again corrected by taking into account the pressure minus rgh.

HTML Code:
`phi -= p_rghEqn.flux();`
In the last step the velocity is reconstructed from the flux

HTML Code:
`U -= rAU*fvc::reconstruct((buoyancyPhi + p_rghEqn.flux())/rAUf);`
and p_rgh is updated

HTML Code:
` p_rgh = p - rhok*gh;`
I do not understand the components of the flux. If they are added we obtain

HTML Code:
`phi = fvc::interpolate(U) & mesh.Sf() - (rAUf*ghf*fvc::snGrad(rhok)*mesh.magSf()) - p_rghEqn.flux();`
So the term including the normal gradient of the density is too much.
http://openfoamwiki.net/index.php/Bu...sinesqPisoFoam

in the solver BuoyantBoussinesqPisoFoam the flux looks like this

HTML Code:
`phi =fvc::interpolate(U) & mesh.Sf()) + rUAf*fvc::interpolate(rhok)*(g & mesh.Sf())-pEqn.flux();`
which makes much more sense to me.
I can not find any explanation in the forum. Who can help me to understand the code?
Attached Images
 Bildschirmfoto.png (9.6 KB, 170 views)

 September 5, 2011, 08:58 #2 Senior Member   Anne Gerdes Join Date: Aug 2010 Location: Hamburg Posts: 168 Rep Power: 11 No one for an answer???

 September 5, 2011, 09:39 #3 Senior Member     Roman Thiele Join Date: Aug 2009 Location: London, UK Posts: 371 Rep Power: 16 I am not sure, but you might have to look up in a numerical methods book, or somewhere else how the SIMPLE algorithm works, maybe that can give you some hints. __________________ ~roman

 September 8, 2011, 09:20 #4 Senior Member   Anne Gerdes Join Date: Aug 2010 Location: Hamburg Posts: 168 Rep Power: 11 Thank you for answering! Now I understand the implementation. If someone is interested I could post that, too.

 September 8, 2011, 11:24 #5 Senior Member   Bernhard Join Date: Sep 2009 Location: Delft Posts: 790 Rep Power: 17 If it is not on this forum yet, then it can be very interesting for future reference if you post your findings here!

 September 12, 2011, 09:02 #6 Senior Member   Anne Gerdes Join Date: Aug 2010 Location: Hamburg Posts: 168 Rep Power: 11 In the momentum equation we have in z-direction (in direction of buoyancy) the terms - dp / dz + rho*g In OpenFOAM, g is a vector (0 0 -9,81) which ensures that the buoyancy is only valid for the right coordinate direction. In order to guarantee, that in the pressure correction of the simple algorithm also the buoyancy term rho*g*z is taken into account, the pressure and the buoyancy are melted together in one term p_rgh = p - rho*g*z Instead of the normal gradient of p, the normal gradient of p_rgh is on the RHS. - d/dn (p_rgh) which equals in OF to HTML Code: ` - fvc :: snGrad (p_rgh)` Computing the derivative of this term with product rule and assuming that rho may change with respect to the z-direction we obtain - d/dz [ p - rho * g *z] = - dp/dz + rho*g + g*z* d rho/dz So the third term g*z* d rho/dz is "too much" and is therefore substracted via HTML Code: `- ghf *fvc::snGrad(rhok)` So the derivative of the density is a correction term which is nonzero for changes in density. klilla, francescomarra, romant and 9 others like this.

 September 14, 2011, 02:08 #7 Senior Member   Dr. Alexander Vakhrushev Join Date: Mar 2009 Posts: 247 Blog Entries: 1 Rep Power: 15 Hallo Anne! Would you please clarify following points: 1. What do you mean by term "two much" (is it phisical meaning or regards difference in some mathematical formulation). 2. Did you use some reference to understand SIMPLE/PISO treatment of the buoyancy? Thank you in advance! Mfg, Alexander Tobi likes this. __________________ Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Metallurgical Applications of Magnetohydrodynamics" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben http://smmp.unileoben.ac.at

 September 14, 2011, 03:47 #8 Senior Member   Anne Gerdes Join Date: Aug 2010 Location: Hamburg Posts: 168 Rep Power: 11 Hallo Alexander, I will try to answer your questions: 1. With "too much" I mean the term g*z* d rho/dz which is the result of taking the derivative of - [ p - rho * g *z] in z-direction. It is an additional term due to the product rule. Basically we have the terms - dp / dz + rho*g So by taking the derivative of both, p and rho*g*z we obtain together with the correction term - g*z* d rho/ dz: - d/dz [ p - rho * g *z] - g*z* d rho/ dz= - dp /dz + rho*g + g*z* d rho/ dz - g*z* d rho/ dz = - dp/ dz + rho*g and this is the orignial term in the buoyancy driven momentum equation. In OpenFOAM- code this equals to the right-hand side of the UEqn HTML Code: ` - fvc::snGrad(p_rgh) - ghf*fvc::snGrad(rhok)` 2. I have a lecture script where this method is described, but it is not open for everyone. I also found a notice for this method in Peric and Ferziger's "Computational Methods for Fluid Dynamics" at the very beginning of the book (page 11 in the version I have). Search for "hydrostatic pressure" and you will find a short explanation there. gaza, MajidHagh and randolph like this.

 September 14, 2011, 04:16 #9 Senior Member   Dr. Alexander Vakhrushev Join Date: Mar 2009 Posts: 247 Blog Entries: 1 Rep Power: 15 Thank you Anne for the detailed explanation! I will search for the algorithm description in Peric's book. Got it, thanx) __________________ Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Metallurgical Applications of Magnetohydrodynamics" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben http://smmp.unileoben.ac.at

 June 8, 2019, 05:27 rhok in T and U equation #10 New Member   siamak rafizadeh Join Date: May 2018 Posts: 8 Rep Power: 3 Hi As anyone knows in buossinesq approximation for density is written as : rho=rhoRef*(1-beta*(T-Tref)) and in oF rhok=1-beta*(T-Tref) and in Chalmer university file: Cite as: Venkatesh, B V.: Tutorial of convective heat transfer in a vertical slot. In Proceedings of CFD with OpenSource Software, 2016, Edited by Nilsson. H., http://www.tfd.chalmers.se/~hani/kurser/OS_CFD_2016 CFD with OpenSource software A course at Chalmers University of Technology Taught by Håkan Nilsson we have: The governing equation for temperature is solved, given as ∇.(ρuT ) − ∇.αef f ∇T = Sradiation + ST (2.4) Where, αef f = νt /prt + ν/pr , Sradiation and ST are source terms due to radiation and user defined source term respectively. The density is updated as ρ = 1 − β(T − Tref ) and phi is defined as phi=rhok*U now question is how rhoRef is deleted in above equstion while alpha have it: α=k/(ρ*Cp) please help in making it clear. thanks in advance

 March 22, 2020, 06:58 #11 New Member   Annabel Parker Join Date: Feb 2020 Posts: 2 Rep Power: 0 In the pressure correction of the simple algorithm also the buoyancy term rho*g*z is taken into account, the pressure and the buoyancy are melted together in one term rufus Last edited by strohl; March 23, 2020 at 02:32. Reason: spelling

 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 tommymoose ANSYS Meshing & Geometry 0 August 5, 2011 16:02 Mechstud Main CFD Forum 4 July 26, 2011 12:13 challenger85 CFX 5 November 5, 2009 05:44 tehache OpenFOAM Running, Solving & CFD 3 July 27, 2007 06:02 Micha Siemens 0 August 6, 2003 13:55

All times are GMT -4. The time now is 01:09.