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

BoussinesqApproximation for incompressible flow

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 12, 2005, 10:30
Default You must either move the g
  #1
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
You must either move the

g*alpha*(T-TRef)

term into the UEqn construction statement

fvVectorMatrix UEqn
...

or also include the term in the flux prediction by including it in

U = UEqn.H()/A;

and remove it from the momentum correction statement

U -= fvc::grad(p)/A + (g*alpha*(T-TRef))/A;
henry is offline   Reply With Quote

Old   June 9, 2006, 16:21
Default Christian, have you had any lu
  #2
ccless
Guest
 
Posts: n/a
Christian, have you had any luck? I have been thinking about a boussinesq solver, but haven't had enough time to write it. Does yours work and if so, what tricks did you use to get it up and running. Thanks
  Reply With Quote

Old   August 2, 2006, 09:36
Default Hi, we also want to build a
  #3
mkk
Guest
 
Posts: n/a
Hi,

we also want to build a boussinesq-approximation.
You wrote your solver in the version 1.2. Am I right?
We changed your idea, so it could work in 1.3.
But we had a problem with the line:
g*alpha*(T-TRef)
what type is TRef and T and where you definded it?

Thanks Martin
  Reply With Quote

Old   February 16, 2007, 12:34
Default Hi, also trying to get an i
  #4
Senior Member
 
Thomas Jung
Join Date: Mar 2009
Posts: 100
Rep Power: 8
tehache is on a distinguished road
Hi,

also trying to get an incompressible boussinesq-approx. solver running ...
I got something working, basically what Christian has posted, with the corrections by Henry.
Works mostly, but sometimes I get problems at boundaries (using a zeroGradient B.C. for pressure) I thought I needed a pressure boundary condition, and implemented one similar to the existing wallBuoyantPressure - just computing the pressure gradient as g*beta*(T-TRef)
Also at first glance seemed to work, gives a smooth looking pressure field, but then I realized strange vectors and pressures at the pressure reference cell, finally calculations diverge. Fixing pressure at some boundary, instead of using pEqn.setReference(pRefCell, pRefValue), works. Not setting a pressure reference the pressure solver (AMG or ICCG) diverges.

almost forgot - using OpenFOAM 1.3

Any hint would be greatly appreciated...

Thank you !

Thomas
tehache is offline   Reply With Quote

Old   March 17, 2007, 15:23
Default For the lazy ones out there, I
  #5
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,763
Rep Power: 21
hjasak will become famous soon enough
For the lazy ones out there, I have written a Boussinesq approximation incompressible buoyant flow solver with constant material properties. You can get it from the link below, including a tutorial case:

boussinesqBuoyantFoam

Currently, it is laminar and quite easy to understand, it will swallow the wall bouyant pressure b.c. and I think it's a pretty decent example. Extensions to turbulent, real material properties etc are straightforward but uninteresting (for me!).

Enjoy,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   March 17, 2007, 18:19
Default This link is dead.
  #6
Member
 
rafal zietara
Join Date: Mar 2009
Location: Manchester, UK
Posts: 60
Rep Power: 8
rafal is on a distinguished road
This link is dead.
rafal is offline   Reply With Quote

Old   March 17, 2007, 19:26
Default Stupid, sorry: boussinesqBuoya
  #7
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,763
Rep Power: 21
hjasak will become famous soon enough
Stupid, sorry: boussinesqBuoyantFoam

Apologies,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   May 16, 2007, 09:19
Default Hrvoje, From one of the laz
  #8
Senior Member
 
Thomas Jung
Join Date: Mar 2009
Posts: 100
Rep Power: 8
tehache is on a distinguished road
Hrvoje,

From one of the lazy ones:

Your implementation suffers the same problems (mass conservation fluxes at walls not parallel to gravity and not at reference temperature).
You can see it if you make your cavity hot at bottom, cold on top, and adiabatic sidewalls.

A pressure B.C. computing pressure gradient as g*beta*(T-TRef), but without contribution to mass fluxes, works.

There is also no need to have an extra density field - which for me is the main point of the Boussinesq approximation.

regards,

Thomas
tehache is offline   Reply With Quote

Old   March 7, 2008, 09:01
Default Hrvoje, we tried to get your
  #9
New Member
 
sonia esteban
Join Date: Mar 2009
Posts: 12
Rep Power: 8
gmc_salta is on a distinguished road
Hrvoje,
we tried to get your Boussinesq approximation incompressible buoyant flow solver, but we get the following message
The page cannot be found
We wait your help...

Sonia
gmc_salta is offline   Reply With Quote

Old   March 7, 2008, 13:36
Default Sorry, probably got deleted: t
  #10
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,763
Rep Power: 21
hjasak will become famous soon enough
Sorry, probably got deleted: try it from SVN:

http://openfoam-extend.svn.sourceforge.net/viewvc/openfoam-extend/trunk/Core/Ope nFOAM-1.4.1-dev/applications/solvers/heatTransfer/boussinesqBuoyantFoam/

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   March 10, 2008, 06:47
Default Hi,Hrvoje Thank you for your
  #11
New Member
 
sonia esteban
Join Date: Mar 2009
Posts: 12
Rep Power: 8
gmc_salta is on a distinguished road
Hi,Hrvoje
Thank you for your help, We can download your files.
We start working on this case.
Sonia
gmc_salta is offline   Reply With Quote

Old   August 13, 2008, 09:41
Default Hi, somebody created a bous
  #12
Senior Member
 
Tian
Join Date: Mar 2009
Location: Berlin, germany
Posts: 103
Rep Power: 8
tian is on a distinguished road
Hi,

somebody created a boussinesq approximation solver with turbulent already and can share it with me? Thanks a lot.

Bye
__________________
BIM HVACTool, The Green Building Simulation Tool for OpenFOAM, Energy Plus and Radiance.
tian is offline   Reply With Quote

Old   August 14, 2008, 16:53
Default Yes: have a look at: http:/
  #13
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,763
Rep Power: 21
hjasak will become famous soon enough
Yes: have a look at:

http://openfoam-extend.svn.sourceforge.net/viewvc/openfoam-extend/trunk/Core/Ope nFOAM-1.4.1-dev/applications/solvers/heatTransfer/boussinesqBuoyantFoam/
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   August 15, 2008, 03:23
Default Hi Hrvoje, this solver is f
  #14
Senior Member
 
Tian
Join Date: Mar 2009
Location: Berlin, germany
Posts: 103
Rep Power: 8
tian is on a distinguished road
Hi Hrvoje,

this solver is for buoyancy-driven laminar flow. I like to try the boussinesq approximation with turbulent flow.

thanks
__________________
BIM HVACTool, The Green Building Simulation Tool for OpenFOAM, Energy Plus and Radiance.
tian is offline   Reply With Quote

Old   August 15, 2008, 05:14
Default Hi Thomas, I just wrote Wik
  #15
Member
 
Masashi IMANO
Join Date: Mar 2009
Location: Tokyo, Japan
Posts: 34
Rep Power: 8
imano is on a distinguished road
Hi Thomas,

I just wrote Wiki page of Boussinesq-Approximation solver for turbulent flow.

http://openfoamwiki.net/index.php/Co...yantSimpleFoam

Also I wrote Wiki page of tutorial case using this solver.

http://openfoamwiki.net/index.php/Ma...onditionedRoom

Bye!

Masashi
imano is offline   Reply With Quote

Old   August 15, 2008, 05:46
Default Hi Masashi, thanks a lot! A
  #16
Senior Member
 
Tian
Join Date: Mar 2009
Location: Berlin, germany
Posts: 103
Rep Power: 8
tian is on a distinguished road
Hi Masashi,

thanks a lot! Arigato

Bye
__________________
BIM HVACTool, The Green Building Simulation Tool for OpenFOAM, Energy Plus and Radiance.
tian is offline   Reply With Quote

Old   August 15, 2008, 08:02
Default Hi Masashi, nice work! I like
  #17
Senior Member
 
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 10
braennstroem is on a distinguished road
Hi Masashi,
nice work! I like your tutorial with the makefile and the python meshing :-)

Fabian
braennstroem is offline   Reply With Quote

Old   August 18, 2008, 10:04
Default Hi Masashi, I have a quest
  #18
Senior Member
 
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 10
braennstroem is on a distinguished road
Hi Masashi,

I have a question about your implementation of the temperature
equation. As I get it, you add a defined heat flux to the equation,
which is activated by the internal field of Q!? I tried a more general
approach by defining a heat flux b.c. using:

const boussinesq::RASModel& RAS = db().lookupObject<boussinesq::rasmodel>("RASProper ties");

scalarField nuEffWall = RAS.nuEff()().boundaryField()[patch().patch().index()];
scalarField alphaEffWall = nuEffWall /Prt;
gradient()=(heatFlux_/(Cp0*rho0*alphaEffWall));

Based on your added b.c. one could use:

wall
{
type fixedHeatFlux;
heatFlux 5.0;
gradient uniform 200;
}

Though I am not sure yet, how to validate this b.c. with a really simple
setup!? And right now, it is a static Prt, Cp0 and rho
implementation. Does anyone know, how to get those value by a
dictionary?




I got one more question about the wall function. Is it correct, that as
long as one uses a constant Pr model is used, the wall effects are all
included in the turbulence model and no separate treatment for the
temperature near-wall behavior is needed?

Fabian
braennstroem is offline   Reply With Quote

Old   August 18, 2008, 11:42
Default Hi Fabian, It seems that f
  #19
Member
 
Masashi IMANO
Join Date: Mar 2009
Location: Tokyo, Japan
Posts: 34
Rep Power: 8
imano is on a distinguished road
Hi Fabian,

It seems that fixedHeatFluxFvPatchScalarField.[C,H] are not attached
properly in your previous post. So please attach them again!

Masashi
imano is offline   Reply With Quote

Old   August 18, 2008, 13:21
Default oh http://www.cfd-online.c
  #20
Senior Member
 
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 10
braennstroem is on a distinguished road
oh

fixedHeatFluxFvPatchScalarField.C
fixedHeatFluxFvPatchScalarField.H
braennstroem 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
boussinesqapproximation mkk OpenFOAM Running, Solving & CFD 0 August 2, 2006 09:32
convert compressible flow into incompressible flow Hun Jung Main CFD Forum 4 August 11, 2003 10:10
AMR with Incompressible Flow Shahriar Main CFD Forum 7 March 7, 2003 09:53
Incompressible Flow A.M.Yang Main CFD Forum 1 July 3, 2002 07:58
How to set BC of incompressible flow zhwm FLUENT 5 February 7, 2002 22:44


All times are GMT -4. The time now is 16:14.