
[Sponsors] 
January 9, 2014, 23:23 
fluent continuity convergence problem

#1 
New Member
Join Date: Jan 2014
Posts: 5
Rep Power: 4 
Hello all,
I have convergence problem in continuity... it's very simple geometry but it is not converge. My geometry is rectangular duct with partially supplying constant heat flux in 2D. I used coupled solver. I think mesh quality and boundary condition are not wrong. I don't know why this problem occurs. Last edited by pibea; January 10, 2014 at 22:12. 

January 10, 2014, 00:20 

#2 
Member
EMAVI V SURYA SAMPATH
Join Date: Aug 2011
Location: Malaysia
Posts: 83
Rep Power: 6 
what is your outlet condition ? if its outflow, try changing to pressure outlet.
and, check your convergence based on mass balance or any other parameter. don't base only on residuals. 

January 10, 2014, 00:21 

#3 
Member
EMAVI V SURYA SAMPATH
Join Date: Aug 2011
Location: Malaysia
Posts: 83
Rep Power: 6 
also, try reducing the URF's of energy, momentum to 0.4...
pressure URF increase to 0.6 post the update if you try these.. 

January 10, 2014, 00:46 
Hi sampathevs, Thank you for your reply:D

#4 
New Member
Join Date: Jan 2014
Posts: 5
Rep Power: 4 
Hi sampathevs, Thank you for your reply
In my geometry, I used pressure outlet and its pressure is 1bar. I change the URF as you recommanded and residuals look more stable. Mass flow rates of inlet and outlet are almost same and other parameters are normal, I think. Then, can I think this case is converge although continuity residual is about 8*10^1? 

January 10, 2014, 03:13 

#5 
Member
EMAVI V SURYA SAMPATH
Join Date: Aug 2011
Location: Malaysia
Posts: 83
Rep Power: 6 
i suppose, yes.!!!


January 10, 2014, 07:51 

#6 
Senior Member
Bharath kumar
Join Date: Apr 2009
Posts: 168
Rep Power: 9 
hi pibea,
I think there may be some basic mistakes may be there. 1. Please check your scale of the mesh. 2. Try first Kepsilon model then switch to RSM (first order). 3. Post some pics to under stand better 

January 10, 2014, 21:54 

#7 
New Member
Join Date: Jan 2014
Posts: 5
Rep Power: 4 
hi bharath,
thank you for your reply. I did not quite understand 'check scale of the mesh' in your reply. Could you please explain that more? Does scale of the mesh mean mesh quality? 

January 10, 2014, 23:30 

#8 
Senior Member
Join Date: Feb 2013
Location: Germany
Posts: 172
Rep Power: 14 
I would advise you to check physical quantities to determine if your solution is ok or nonsense. Do they change over the number of iterations after the residuals seem to be converged? If available compare to experimental data. For such simple cases it is often possible to do some analytical calculation and compare it to your results.
The mass residual can be missleading sometimes as it is scaled (divided by) the maximum residual of iteration 1 to 5. Fluent plots this scaled residual. If the maximum residual iteration 1 to 5 is already pretty low, the scaled residual will take large values. This would be typical for a interpolated case or a good initial guess. It could also be possible that mass residual iteration 1 to 5 is already so low that the scaled residual takes large values as it is a very simple case. Further you could try to run the case in double precision. "Check scale" means that the lenght unit in fluent and the lenght unit of your mesh has to be the same otherwise you have to scale your mesh. It is a pretty common mistake to forget scaling. You can run check mesh to display your domain extends in Fluent. As your case is very simple I don't think URFs should be the problem. Also: 

January 11, 2014, 00:28 

#9 
Member
EMAVI V SURYA SAMPATH
Join Date: Aug 2011
Location: Malaysia
Posts: 83
Rep Power: 6 
yea, as bharat said, check the scale of mesh..
General scale check your dimensions, mm or m , cm ..for your geometry 

February 13, 2014, 18:42 

#10 
New Member
shaham
Join Date: Feb 2011
Posts: 5
Rep Power: 7 
Hi,
I found a convergence problem in Fluent 15. I tried a simple 3D pipe model which I was using in fluent 14 and it had no problem in converging, however, in 15 the same case I use have the problem with the continuity. I also tried the same 2D axisymetric case, and in version 15 it takes about 30% more iteration to converge the same conditions. I wonder if anyone had this problem and if there is any solution for this problem? Thanks 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Fluent Mixed Convection Problem  cfdsolver1  FLUENT  2  May 14, 2014 23:52 
Micro Scale Pore, icoFoam  gooya_kabir  OpenFOAM Running, Solving & CFD  2  November 2, 2013 14:58 
Can I solve this problem by Fluent?  Kai_kc  FLUENT  1  October 27, 2010 05:29 
Convergence moving mesh  lr103476  OpenFOAM Running, Solving & CFD  30  November 19, 2007 15:09 
IcoFoam parallel woes  msrinath80  OpenFOAM Running, Solving & CFD  9  July 22, 2007 02:58 