CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

fluent continuity convergence problem

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 9, 2014, 23:23
Default fluent continuity convergence problem
  #1
New Member
 
Join Date: Jan 2014
Posts: 5
Rep Power: 3
pibea is on a distinguished road
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.
Attached Images
File Type: jpg help.jpg (57.7 KB, 82 views)

Last edited by pibea; January 10, 2014 at 22:12.
pibea is offline   Reply With Quote

Old   January 10, 2014, 00:20
Default
  #2
Member
 
EMAVI V SURYA SAMPATH
Join Date: Aug 2011
Location: Malaysia
Posts: 83
Rep Power: 5
sampathevs is on a distinguished road
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 is offline   Reply With Quote

Old   January 10, 2014, 00:21
Default
  #3
Member
 
EMAVI V SURYA SAMPATH
Join Date: Aug 2011
Location: Malaysia
Posts: 83
Rep Power: 5
sampathevs is on a distinguished road
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..
sampathevs is offline   Reply With Quote

Old   January 10, 2014, 00:46
Default Hi sampathevs, Thank you for your reply:D
  #4
New Member
 
Join Date: Jan 2014
Posts: 5
Rep Power: 3
pibea is on a distinguished road
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?
Attached Images
File Type: jpg help2.jpg (59.1 KB, 71 views)
pibea is offline   Reply With Quote

Old   January 10, 2014, 03:13
Default
  #5
Member
 
EMAVI V SURYA SAMPATH
Join Date: Aug 2011
Location: Malaysia
Posts: 83
Rep Power: 5
sampathevs is on a distinguished road
i suppose, yes.!!!
sampathevs is offline   Reply With Quote

Old   January 10, 2014, 07:51
Default
  #6
Senior Member
 
Bharath kumar
Join Date: Apr 2009
Posts: 157
Rep Power: 8
bharath is on a distinguished road
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
bharath is offline   Reply With Quote

Old   January 10, 2014, 21:54
Default
  #7
New Member
 
Join Date: Jan 2014
Posts: 5
Rep Power: 3
pibea is on a distinguished road
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?
pibea is offline   Reply With Quote

Old   January 10, 2014, 23:30
Default
  #8
kad
Senior Member
 
Join Date: Feb 2013
Location: Germany
Posts: 171
Rep Power: 13
kad will become famous soon enoughkad will become famous soon enough
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:
Quote:
Originally Posted by bharath View Post
hi pibea,
Try first K-epsilon model (or other model) then switch to RSM (first order).
kad is offline   Reply With Quote

Old   January 11, 2014, 00:28
Default
  #9
Member
 
EMAVI V SURYA SAMPATH
Join Date: Aug 2011
Location: Malaysia
Posts: 83
Rep Power: 5
sampathevs is on a distinguished road
yea, as bharat said, check the scale of mesh..

General-- scale

check your dimensions, mm or m , cm ..for your geometry
sampathevs is offline   Reply With Quote

Old   February 13, 2014, 18:42
Default
  #10
New Member
 
shaham
Join Date: Feb 2011
Posts: 3
Rep Power: 6
shaham is on a distinguished road
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
shaham 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
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


All times are GMT -4. The time now is 13:42.