CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Convergence (http://www.cfd-online.com/Forums/fluent/32245-convergence.html)

eric October 2, 2003 04:56

Convergence
 
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.

ap October 2, 2003 07:55

Re: Convergence
 
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

eric October 3, 2003 04:57

Re: Convergence
 
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

ap October 3, 2003 15:00

Re: Convergence
 
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

eric October 4, 2003 06:38

Re: Convergence
 
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

eric October 4, 2003 09:50

Re: Convergence
 
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

ap October 4, 2003 11:16

Re: Convergence
 
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.

eric October 31, 2003 12:55

Re: Convergence
 
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

ap October 31, 2003 13:25

Re: Convergence
 
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

eric November 1, 2003 07:01

Re: Convergence
 
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

ap November 1, 2003 08:34

Re: Convergence
 
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

ap November 1, 2003 08:54

Re: Convergence
 
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

eric November 1, 2003 10:32

Re: Convergence
 
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

ap November 1, 2003 11:15

Re: Convergence
 
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

eric November 1, 2003 11:57

Re: Convergence
 
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


All times are GMT -4. The time now is 18:31.