|
[Sponsors] |
Cavity Benchmark - buoyantBoussinesqSimpleFoam - poor Nu |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
February 9, 2015, 08:11 |
Cavity Benchmark - buoyantBoussinesqSimpleFoam - poor Nu
|
#1 |
Member
Thiago Parente Lima
Join Date: Sep 2011
Location: Diamantina, Brazil.
Posts: 62
Rep Power: 14 |
Hi all,
I'm trying to solve the problem of a square cavity heated and coole at the vertical walls using the buoyantBoussinesqsimpleFoam. The problem converges well and the results are qualitatively ok. I have two problems: - When I calculate the average Nusselt at the cold wall and compare against the benchmark solution by DeVahl (1983) the results are quite poor. - I solved the problem for Ra = 10³, Pr = 0.71 for a cavity of length 1m (100x100 grid) modifying the gravitty vector accordingly, then when I solve the same problem setting g=-9.81 and modifying the cavity length to get Ra=10³, I obtain a different Nusselt number!! I solved this problem using a FORTRAN package (90x90 grid) and the results are pretty good (Nu=1.118). The Nusselt number for the FORTRAN results are calculated in the same way as the OpenFoam case (same file!), so the problem is not there. Now, I don't know what am I doing wrong. Older threads in this forum did not help me. My case is attached and I would appreciate if somebody could help me. https://drive.google.com/file/d/0BypOSbibeu1nZlZyQVotQjBDM0k/view?usp=sharing Note: if the link doesn't work, copy paste the address. |
|
February 9, 2015, 10:55 |
|
#2 |
Senior Member
Nima Samkhaniani
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,266
Blog Entries: 1
Rep Power: 24 |
1- did you try grid independence test? maybe you need much more refined cells near wall
2- did you use second order schemes?
__________________
My Personal Website (http://nimasamkhaniani.ir/) Telegram channel (https://t.me/cfd_foam) |
|
February 9, 2015, 12:11 |
|
#3 |
Member
Thiago Parente Lima
Join Date: Sep 2011
Location: Diamantina, Brazil.
Posts: 62
Rep Power: 14 |
Hi nimasam,
Thank you for your attetion. 1. Yes, I did. The variation in Nu is of 0,4% from a 100x100 to a 140x140 uniform grid. Nu=1,982 (!!) for 140x140 (this authors reported Nu=1,109 for 100x100 using the same solver and schemes). 2. Yes. I used bound Gauss QUICK for divSchemes in div(phi,U) and div(phi,T), the rest remains the same as the problem is laminar (the turbulence is off in RASproperties). Also, I used a forward second order scheme to calculate Nu at the cold wall and trapezoidal rule to integrate. I defined Teta = (T-Th)/(Th-Tc), X=x/L, then Nu = Int_0_1(dTeta/dX). Th=301, Tc=300, L=1. The BC are: - p and p_rgh are the same of the horRoom tutorial. - T fixedValue (hot and cold wall) and zeroGradient (adiabatic walls) - U fixedValue (0,0,0), no slip. |
|
February 9, 2015, 14:32 |
|
#4 |
Member
Thiago Parente Lima
Join Date: Sep 2011
Location: Diamantina, Brazil.
Posts: 62
Rep Power: 14 |
I think I found the reason why the Nu differs even when I run the cases with the same Ra and Pr (although it makes no sense). If I run the case 1 (Ra=10³ w/ L=1, g=4.6e-5) and case 2 (Ra=10³ w/ L=0.016, g=9.81), both give the same Nu (as it should) if I start the simulation from uniform initial fields.
The problem appears, for example, when I run case 1 using mapFields from a coarser grid. The problem coverges, but it results in a Nu that differs from the case 2 solved without mapFields. Summarizing: A case with the same Ra and Pr gives different converged solutions depending on its initial fields (!!). Of course it makes no sense, but why it could be happen? |
|
February 9, 2015, 15:59 |
|
#5 |
Senior Member
Nima Samkhaniani
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,266
Blog Entries: 1
Rep Power: 24 |
How about your fvSolution, you may want to reduce your convergence criteria
__________________
My Personal Website (http://nimasamkhaniani.ir/) Telegram channel (https://t.me/cfd_foam) |
|
February 10, 2015, 12:38 |
|
#6 |
Member
Thiago Parente Lima
Join Date: Sep 2011
Location: Diamantina, Brazil.
Posts: 62
Rep Power: 14 |
Hi nimasam,
In fact the SIMPLE residualControl was low, so I changed as shown below. Code:
solvers { p_rgh { solver PCG; preconditioner DIC; tolerance 1e-08; relTol 0.01; } "(U|T|k|epsilon|R)" { solver PBiCG; preconditioner DILU; tolerance 1e-05; relTol 0.01; } } SIMPLE { nNonOrthogonalCorrectors 0; pRefCell 0; pRefValue 0; residualControl { p_rgh 1e-5; U 1e-5; T 1e-5; // possibly check turbulence fields "(k|epsilon|omega)" 1e-3; } } I also notice that the No Iterations for Ux and Uy is never more than 2 (it reachs 0 as the problems converge). The residuals for Ux, Uy and T fall rapidly, but it seems strange, don't you think? It should be a simple problem... Last edited by thiagopl; February 10, 2015 at 13:33. Reason: Attached figure |
|
February 10, 2015, 23:07 |
|
#7 |
Senior Member
Nima Samkhaniani
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,266
Blog Entries: 1
Rep Power: 24 |
convergence does not mean correct answer , i suggest:
1-reduce relTol to zero 2-use linearUpwind
__________________
My Personal Website (http://nimasamkhaniani.ir/) Telegram channel (https://t.me/cfd_foam) |
|
February 11, 2015, 07:46 |
|
#8 |
Member
Thiago Parente Lima
Join Date: Sep 2011
Location: Diamantina, Brazil.
Posts: 62
Rep Power: 14 |
Sure, actually, convergence doesn't mean it's the end of your problems.
It seems that the problem is in fvSolutions. I'll make some changes, see the results and post when something good happens. I have one question about the tolerance and the residualControl, is there one that prevails over the other or they are verified in different points during the solution process? Thank you! Last edited by thiagopl; February 11, 2015 at 07:48. Reason: English |
|
February 11, 2015, 13:47 |
|
#9 |
Senior Member
Nima Samkhaniani
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,266
Blog Entries: 1
Rep Power: 24 |
Residual control just checks initial residuals, and if the value of initial residual for all variables become below the criteria, it will stop.
__________________
My Personal Website (http://nimasamkhaniani.ir/) Telegram channel (https://t.me/cfd_foam) |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Urgent: Unsteady 3-D supersonic cavity flow | Min-Sung Kang | FLUENT | 3 | April 6, 2014 09:50 |
Benchmark data for temperature field in 2D cavity flow | Vladislav | Main CFD Forum | 0 | June 18, 2010 12:33 |
cavity in flat plate and drag prediction | Far | FLUENT | 0 | May 19, 2010 14:47 |
To those who are looking for 2D cavity benchmark | wuliang | Main CFD Forum | 2 | August 3, 2006 05:17 |
Benchmark (Lid driven cavity, ...) | rt | Main CFD Forum | 3 | April 1, 2006 09:27 |