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

BuoyantBoussinesq(Pimple/Piso)Foam, changed equation from OF 1.6 to 1.7 ???

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 27, 2010, 10:37
Default BuoyantBoussinesq(Pimple/Piso)Foam, changed equation from OF 1.6 to 1.7 ???
  #1
New Member
 
Jan
Join Date: Jun 2010
Location: Erlangen, Germany
Posts: 3
Rep Power: 7
myself is on a distinguished road
Hi Folks,

one question regarding the changes from OF 1.6 to 1.7 in the buoyantBoussinesq(Piso/Pimple)Foam solver. I think the implementation of splitting the pressure according to p = p_rgh + rho*g.x is not fully correct.

The pressure equation in OF 1.7 seems OK, since in the Rhie-Chow formulation the contributions from the static pressure cancel and we are left with:
Code:
phi = (fvc::interpolate(U) & mesh.Sf())
        + fvc::ddtPhiCorr(rUA, U, phi);

surfaceScalarField buoyancyPhi = rUAf*ghf*fvc::snGrad(rhok)*mesh.magSf();
phi -= buoyancyPhi;
instead of
Code:
 surfaceScalarField phiU
    (
        (fvc::interpolate(U) & mesh.Sf())
      + fvc::ddtPhiCorr(rUA, U, phi)
    );

    phi = phiU + rUAf*fvc::interpolate(rhok)*(g & mesh.Sf());
in OF 1.6.

In contrast, in the momentum equation the term for the buoyancy ( and gravity) force has changed from (OF 1.6)
Code:
fvc::reconstruct( ...
                    fvc::interpolate(rhok)*(g & mesh.Sf())  ...)
to (OF 1.7)
Code:
fvc::reconstruct( ...
  - ghf*fvc::snGrad(rhok)*mesh.magSf() ...)
These are two different expressions: F ~ rhok * g vs. F ~ gradT * g.h

Is this really a bug or do I miss some point? Thanks for any comment...

Regards,
Jan


Edit:
In the meantime I am pretty sure this is indeed a bug and I submitted a bugreport.

Edit:
Problem is solved. This bug was fixed a few days ago in the git repository.

Last edited by myself; October 7, 2010 at 11:19.
myself is offline   Reply With Quote

Old   July 28, 2011, 05:21
Default
  #2
Senior Member
 
Anne Gerdes
Join Date: Aug 2010
Location: Hamburg
Posts: 152
Rep Power: 7
Anne Lincke is on a distinguished road
Dear Foamers,
can someone explain me why OF1.7 still uses

HTML Code:
- ghf*fvc::snGrad(rhok)*mesh.magSf()
instead of

HTML Code:
fvc::interpolate(rhok)*(g & mesh.Sf())
as it was used in the previous version OF1.6.
I do not understand why the gradient of the densitiy is used while in the equations I find in literature it has to be just the densitiy multiplied with the constant g.
Can someone help me? Is this still a bug or do I overlook something?
Anne Lincke is offline   Reply With Quote

Old   September 13, 2011, 08:38
Default
  #3
Senior Member
 
Anne Gerdes
Join Date: Aug 2010
Location: Hamburg
Posts: 152
Rep Power: 7
Anne Lincke is on a distinguished road
For the answer see

Problems in understanding BuoyantBoussinesqSimpleFoam
Anne Lincke is offline   Reply With Quote

Old   September 14, 2011, 02:03
Default
  #4
Senior Member
 
Dr. Alexander Vakhrushev
Join Date: Mar 2009
Posts: 213
Rep Power: 10
makaveli_lcf is on a distinguished road
Send a message via ICQ to makaveli_lcf
Quote:
Originally Posted by myself View Post
Hi Folks,

one question regarding the changes from OF 1.6 to 1.7 in the buoyantBoussinesq(Piso/Pimple)Foam solver. I think the implementation of splitting the pressure according to p = p_rgh + rho*g.x is not fully correct.

The pressure equation in OF 1.7 seems OK, since in the Rhie-Chow formulation the contributions from the static pressure cancel and we are left with:
Code:
phi = (fvc::interpolate(U) & mesh.Sf())
        + fvc::ddtPhiCorr(rUA, U, phi);

surfaceScalarField buoyancyPhi = rUAf*ghf*fvc::snGrad(rhok)*mesh.magSf();
phi -= buoyancyPhi;
instead of
Code:
 surfaceScalarField phiU
    (
        (fvc::interpolate(U) & mesh.Sf())
      + fvc::ddtPhiCorr(rUA, U, phi)
    );

    phi = phiU + rUAf*fvc::interpolate(rhok)*(g & mesh.Sf());
in OF 1.6.

In contrast, in the momentum equation the term for the buoyancy ( and gravity) force has changed from (OF 1.6)
Code:
fvc::reconstruct( ...
                    fvc::interpolate(rhok)*(g & mesh.Sf())  ...)
to (OF 1.7)
Code:
fvc::reconstruct( ...
  - ghf*fvc::snGrad(rhok)*mesh.magSf() ...)
These are two different expressions: F ~ rhok * g vs. F ~ gradT * g.h

Is this really a bug or do I miss some point? Thanks for any comment...

Regards,
Jan


Edit:
In the meantime I am pretty sure this is indeed a bug and I submitted a bugreport.

Edit:
Problem is solved. This bug was fixed a few days ago in the git repository.
Hallo Jan!

You wrote that the term in OF17 was formulated with an error, am I correct?

But still if i look OF171 (Ubuntu package installed via apt-get):

Code:
            UEqn
         ==
            fvc::reconstruct
            (
                (
                  - ghf*fvc::snGrad(rhok)
                  - fvc::snGrad(p_rgh)
                )*mesh.magSf()
            )
Is this term still there? And how it should be?

Regards,
Alexander
__________________
Best regards,

Dr. Alexander VAKHRUSHEV

Christian Doppler Laboratory for "Advanced Process Simulation of
Solidification and Melting"

Simulation and Modelling of Metallurgical Processes
Department of Metallurgy
University of Leoben

Franz-Josef-Str. 18
A - 8700 Leoben
Österreich / Austria
Tel.: +43 3842 - 402 - 3125
http://smmp.unileoben.ac.at
makaveli_lcf 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
Calculation of the Governing Equations Mihail CFX 7 September 7, 2014 06:27
OpenFOAM 1.6 and 1.7 with interFoam, groovyBC give different strange results Arnoldinho OpenFOAM 7 December 9, 2010 17:29
Constant velocity of the material Sas CFX 15 July 13, 2010 08:56
Compatibility from OF 1.6 to OF 1.7? Chrisi1984 OpenFOAM Installation 2 July 7, 2010 03:07
mass flow in is not equal to mass flow out saii CFX 2 September 18, 2009 08:07


All times are GMT -4. The time now is 13:16.