|
[Sponsors] |
BoussinesqApproximation for incompressible flow |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
July 12, 2005, 11:30 |
You must either move the
g
|
#1 |
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 22 |
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; |
|
June 9, 2006, 17:21 |
Christian, have you had any lu
|
#2 |
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
|
|
August 2, 2006, 10:36 |
Hi,
we also want to build a
|
#3 |
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 |
|
February 16, 2007, 12:34 |
Hi,
also trying to get an i
|
#4 |
Senior Member
Thomas Jung
Join Date: Mar 2009
Posts: 102
Rep Power: 17 |
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 |
|
March 17, 2007, 15:23 |
For the lazy ones out there, I
|
#5 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,902
Rep Power: 33 |
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 |
|
March 17, 2007, 18:19 |
This link is dead.
|
#6 |
Member
rafal zietara
Join Date: Mar 2009
Location: Manchester, UK
Posts: 60
Rep Power: 17 |
This link is dead.
|
|
March 17, 2007, 19:26 |
Stupid, sorry: boussinesqBuoya
|
#7 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,902
Rep Power: 33 |
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk |
|
May 16, 2007, 10:19 |
Hrvoje,
From one of the laz
|
#8 |
Senior Member
Thomas Jung
Join Date: Mar 2009
Posts: 102
Rep Power: 17 |
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 |
|
March 7, 2008, 09:01 |
Hrvoje,
we tried to get your
|
#9 |
New Member
sonia esteban
Join Date: Mar 2009
Posts: 12
Rep Power: 17 |
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 |
|
March 7, 2008, 13:36 |
Sorry, probably got deleted: t
|
#10 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,902
Rep Power: 33 |
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 |
|
March 10, 2008, 06:47 |
Hi,Hrvoje
Thank you for your
|
#11 |
New Member
sonia esteban
Join Date: Mar 2009
Posts: 12
Rep Power: 17 |
Hi,Hrvoje
Thank you for your help, We can download your files. We start working on this case. Sonia |
|
August 13, 2008, 10:41 |
Hi,
somebody created a bous
|
#12 |
Senior Member
Tian
Join Date: Mar 2009
Location: Berlin, germany
Posts: 119
Rep Power: 17 |
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. |
|
August 14, 2008, 17:53 |
Yes: have a look at:
http:/
|
#13 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,902
Rep Power: 33 |
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 |
|
August 15, 2008, 04:23 |
Hi Hrvoje,
this solver is f
|
#14 |
Senior Member
Tian
Join Date: Mar 2009
Location: Berlin, germany
Posts: 119
Rep Power: 17 |
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. |
|
August 15, 2008, 06:14 |
Hi Thomas,
I just wrote Wik
|
#15 |
Member
Masashi IMANO
Join Date: Mar 2009
Location: Tokyo, Japan
Posts: 34
Rep Power: 17 |
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 |
|
August 15, 2008, 06:46 |
Hi Masashi,
thanks a lot! A
|
#16 |
Senior Member
Tian
Join Date: Mar 2009
Location: Berlin, germany
Posts: 119
Rep Power: 17 |
Hi Masashi,
thanks a lot! Arigato Bye
__________________
BIM HVACTool, The Green Building Simulation Tool for OpenFOAM, Energy Plus and Radiance. |
|
August 15, 2008, 09:02 |
Hi Masashi,
nice work! I like
|
#17 |
Senior Member
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 19 |
Hi Masashi,
nice work! I like your tutorial with the makefile and the python meshing :-) Fabian |
|
August 18, 2008, 11:04 |
Hi Masashi,
I have a quest
|
#18 |
Senior Member
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 19 |
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 |
|
August 18, 2008, 12:42 |
Hi Fabian,
It seems that f
|
#19 |
Member
Masashi IMANO
Join Date: Mar 2009
Location: Tokyo, Japan
Posts: 34
Rep Power: 17 |
Hi Fabian,
It seems that fixedHeatFluxFvPatchScalarField.[C,H] are not attached properly in your previous post. So please attach them again! Masashi |
|
August 18, 2008, 14:21 |
oh
http://www.cfd-online.c
|
#20 |
Senior Member
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 19 |
||
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
boussinesqapproximation | mkk | OpenFOAM Running, Solving & CFD | 0 | August 2, 2006 10:32 |
convert compressible flow into incompressible flow | Hun Jung | Main CFD Forum | 4 | August 11, 2003 11:10 |
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 08:58 |
How to set BC of incompressible flow | zhwm | FLUENT | 5 | February 7, 2002 22:44 |