CFD Online Discussion Forums

CFD Online Discussion Forums (
-   FLUENT (
-   -   fluent continuity convergence problem (

pibea January 9, 2014 23:23

fluent continuity convergence problem
1 Attachment(s)
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.

sampathevs January 10, 2014 00:20

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.

sampathevs January 10, 2014 00:21

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..

pibea January 10, 2014 00:46

Hi sampathevs, Thank you for your reply:D
1 Attachment(s)
Hi sampathevs, Thank you for your reply:D
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?

sampathevs January 10, 2014 03:13

i suppose, yes.!!!

bharath January 10, 2014 07:51

hi pibea,
I think there may be some basic mistakes may be there.

1. Please check your scale of the mesh.
2. Try first K-epsilon model then switch to RSM (first order).
3. Post some pics to under stand better

pibea January 10, 2014 21:54

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?

kad January 10, 2014 23:30

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:D. 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.


Originally Posted by bharath (Post 469437)
hi pibea,
Try first K-epsilon model (or other model) then switch to RSM (first order).

sampathevs January 11, 2014 00:28

yea, as bharat said, check the scale of mesh..

General-- scale

check your dimensions, mm or m , cm ..for your geometry

shaham February 13, 2014 18:42


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?


raunakjung March 7, 2017 07:17

Were you able to solve the problems ? If Yes please comment

All times are GMT -4. The time now is 18:28.