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

Convergence

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 2, 2003, 04:56
Default Convergence
  #1
eric
Guest
 
Posts: n/a
Hi all,

I am conducting a steady state combustion simulation in a burner tube using a two step methane mechanism with eddy dissipation model and I'm using the ke turbulence model with standard wall functions.

The simulation starts well with a converging trend. However after approximately 500 iterations and a residual level of e-04 reversed flow at outlet warnings appear and the levels out and some variables start a diverging trend.

What can cause this reverse flow warnings at such a late stage?

I want the species to converge to at least -06, so how can i get this to happen??

Regards,

Eric.
  Reply With Quote

Old   October 2, 2003, 07:55
Default Re: Convergence
  #2
ap
Guest
 
Posts: n/a
First of all check boudary conditions on the BC where you have reversed flow. Make sure turbulence parameters are set properly.

If all settings of your case are ok, try reducing the under relaxation factors of diverging variables and meybe decrease the order of the discretization scheme of the same variables.

Hope this works

Hi

ap
  Reply With Quote

Old   October 3, 2003, 04:57
Default Re: Convergence
  #3
eric
Guest
 
Posts: n/a
Hi ap,

Thanks for the advice. I have another problem.

When i mesh my burner with a boundary layer, in gambit, and try to solve it in fluent it won't converge pass e-04. But if i try to solve the same problem without a boundary layer the residuals converge pass -06.

I know this is not much information but can you tell me why this is happening?

Regards,

Eric
  Reply With Quote

Old   October 3, 2003, 15:00
Default Re: Convergence
  #4
ap
Guest
 
Posts: n/a
Pay attention to your y+ values. They must be between 30 and 60 for wall-functions validity.

Also, maybe your boundary layer creates a sort of alteration in the grid, which affects the stability of the solution. This happens expecially if the boundary layer is a lot finer than the rest of your mesh.

I often met similar problems and usually I solved them removing the boundary layer if not strictly necessary.

Hi

ap
  Reply With Quote

Old   October 4, 2003, 06:38
Default Re: Convergence
  #5
eric
Guest
 
Posts: n/a
Hi ap,

Thanks again for your help.

I have often wondered if a boundary layer is necessary in the simulation. How do you, personally, decide whether or not to add a boundary layer to your models?

Regards,

Eric
  Reply With Quote

Old   October 4, 2003, 09:50
Default Re: Convergence
  #6
eric
Guest
 
Posts: n/a
Also, how do i check the y+ value along a wall?

In fluent - display/contours/turbulence/Y+ and then select the wall i want to check?

Is that how i do it??

Regards,

Eric
  Reply With Quote

Old   October 4, 2003, 11:16
Default Re: Convergence
  #7
ap
Guest
 
Posts: n/a
I think that if your mesh has a good quality, so it's fine enough to capture properties changes at the wall, you don't need a boundary layer.

In my opinion, you should use a boundary layer only of you need a really fine mesh near the wall (for example if you use Enhanced wall-functions, which requires y+ close to 1), or if you have to capture big changes in properties in the same zone.

You can check y+ also using xy plot, by selecting walls.

You can obtain max and min y+ values also from the y+ adaption panel.
  Reply With Quote

Old   October 31, 2003, 12:55
Default Re: Convergence
  #8
eric
Guest
 
Posts: n/a
Hi ap,

When i check my Y+ values in the adaption panel the min value is 0. However when i try to coarse the grid fluent won't do it. I think it's down the hanging node. I there another way of 'coarsing' the grid?

Thanks Eric
  Reply With Quote

Old   October 31, 2003, 13:25
Default Re: Convergence
  #9
ap
Guest
 
Posts: n/a
First of all, you should check where y+ is zero. Just plot y+ on your whole domain. Maybe it happens in a portion of the domain not yet reached by the fluid.

Anyway, to coarsen the grid you have two ways:

1. Use the adaption tool.

2. Re-mesh your domain in GAMBIT.

Hi

ap
  Reply With Quote

Old   November 1, 2003, 07:01
Default Re: Convergence
  #10
eric
Guest
 
Posts: n/a
Hi ap,

No matter what I do my Y+ min is 0.

I set the grid in gambit to 3 and solved the flow and Y+ min is 0. I then change the grid spacing to 0.8 and still Y+ min is 0.

Can you tell me where i'm going wrong?

Regards,

Eric
  Reply With Quote

Old   November 1, 2003, 08:34
Default Re: Convergence
  #11
ap
Guest
 
Posts: n/a
Hi eric,

it's difficult to answer without having the case file. Seems strange y+ doesn't change with the grid spacing.

However, try plotting y+ selecting all default-interiors of your domain. This allows you to understand in which part of the domain you have y+ = 0.

A single cell or a small group of cells with y+ = 0 gives you a minimum y+ equal to zero, and this surely is not meaningful.

Also try to complete the calculation to see if results are acceptable (proper form of curves, accepable values...).

What's the max value of y+?

Hi

ap
  Reply With Quote

Old   November 1, 2003, 08:54
Default Re: Convergence
  #12
ap
Guest
 
Posts: n/a
Sorry Eric I made a mistake, I wrote

"However, try plotting y+ selecting all default-interiors of your domain."

I meant selecting "all walls".

Hi

ap
  Reply With Quote

Old   November 1, 2003, 10:32
Default Re: Convergence
  #13
eric
Guest
 
Posts: n/a
Thanks ap,

I've managed to reduce the number of cells under Y+ 20 to 8, which is acceptable.

I have another problem now. On the same grid I'm getting the following error message when i open the grid file in fluent.

Error: access: unbound variable Error Object: phase-domain?

It doesn't seem to have any effect on the simulation. Any idea's??

Eric
  Reply With Quote

Old   November 1, 2003, 11:15
Default Re: Convergence
  #14
ap
Guest
 
Posts: n/a
If it happens when you open the .msh file, and the grid check is ok (I read your other post), it should not be related to your mesh.

Maybe you're opening the mesh file in a previously opened session of FLUENT with data still in memory. Try to quit Fluent, run it again and open the mesh file.

Hi

ap
  Reply With Quote

Old   November 1, 2003, 11:57
Default Re: Convergence
  #15
eric
Guest
 
Posts: n/a
I checked it out on the fluent website. It has to do with how you name your boundaries. For example they should be named inlet_1 or inlet-1 and not inlet 1. A character space causes the problem. Thanks anyway.

My simulation is going well now, Thanks

Eric
  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
Convergence Centurion2011 FLUENT 23 February 18, 2015 15:12
problem with Min/max rho tH3f0rC3 OpenFOAM 7 February 23, 2013 06:37
Force can not converge colopolo CFX 13 October 4, 2011 22:03
Convergence of CFX field in FSI analysis nasdak CFX 2 June 29, 2009 01:17
Defect correction and convergence ganesh Main CFD Forum 4 June 30, 2006 14:20


All times are GMT -4. The time now is 21:21.