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

error in AMG solver

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 1, 2008, 11:59
Default error in AMG solver
  #1
Míša Milakovová
Guest
 
Posts: n/a
Hallo, can anybody help me with next problem - if I try to iterate 3D model two flows, after for about 150 - 200 iteration, Fluent give me next error :

Error : Divergence detected in AMG solver : Temperature Error Object: ()

Thank You !
  Reply With Quote

Old   April 1, 2008, 12:13
Default Re: error in AMG solver
  #2
Julien Lepaul
Guest
 
Posts: n/a
Hi, try to modify the under-relaxation factors in Solve --> Controls --> Solution
  Reply With Quote

Old   April 2, 2008, 00:50
Default Re: error in AMG solver
  #3
Ant
Guest
 
Posts: n/a
Hi

Re-check you boundary and initial conditions and mesh and length scales.

Use Grid-Check and see if the you have properly scaled the model ones the mesh was imported into Fluent.

Check inflow and outflow boundary conditions to see if you have specified proper turbulence parameters. Do not use the standard values of "1". Check if the boundary conditions are just right.

Check the mesh quality in Gambit and Fluent. If you have very skewed elements and the physics is complex, the simulation would crash.

Since the temperature equation is diverging it could be probable that you are using compressible flow or ideal gas equation. If you are using ideal gas, change to incompressble ideal gas for the first few iterations. If you are simulating supersonic flow, start with a lower mass flow at the inlet and slowly ramp up the mass flow rate every 50-100 iterations.

More details can be discussed if you give proper background of your case.

Regards, Ananth
  Reply With Quote

Old   April 2, 2008, 07:35
Default Re: error in AMG solver
  #4
sudhir
Guest
 
Posts: n/a
hi ananth,

just like misa i have same divergence problem. i am simulating solidification of phase material in container.. i have selected only energy no flow under parameters.....can u help me? is it possible to simulate pure conduction problem in fluent? thank you

  Reply With Quote

Old   April 2, 2008, 08:28
Default Re: error in AMG solver
  #5
Ant
Guest
 
Posts: n/a
Are you simulating pure substance or binary metal solidification? Is it continuous casting?

Steady/transient case?

If you are using solidification model you solve for liquid fraction equation and do not explicitly track the solid-liquid interface.

The convergence is difficult for solidification cases due to large temperature gradients. Latent heat is released in the Mushy zone when temperature goes from liquidus to solidus. This is accompanied by step change in momentum source (to stop momentum equation being solved in solid region) and mass source.

Suggestion for the first query would apply to you as well. Make sure mesh is good and turbulence conditions are specified. Try starting without solidification model for first few iterations.

Try changing the value of "Liquid fraction update" in under-relaxation panel.

If this does not help heavy under-relaxation of either energy or "continuity & momentum" would help. I have found that under-relaxation of "momentum & continuity" helps better than under-relaxation of energy. But you would need to figure out which method would suit your case.

Regards, Ant

  Reply With Quote

Old   April 4, 2008, 01:29
Default Re: error in AMG solver
  #6
amol
Guest
 
Posts: n/a
Hi, Anant

I'm Simulating the multiphase model, Secondary Clarifier having 0.4% of solid. I want to see the flow behavior of Particle which approch should be better one eulerian or DPM. DPM model is not converging i used tri as well simply quadra but still not converging will you plz give your suggestion.

Regards, Amol
  Reply With Quote

Old   April 4, 2008, 01:32
Default Re: error in AMG solver
  #7
sudhir
Guest
 
Posts: n/a
hi ant.

thanks for the reply..now my model is converging without any divergence... description of model: a cylindrical tank with its ends insulated.i am changing only the wall temperature.. it is a transient unsteady state problem becoz density varies with temperature.my working fluid is paraffin .fluid is stationery inside the tank. my project is to validate numerical and experimental results.. is it possible to change 1st order upwind scheme to central differencing scheme in "solution -->controls". becoz all my numerical analysis data are based on central differencing scheme? is it possible to change ? or any other way to solve this type of problems in fluent? plz help me....
  Reply With Quote

Old   April 8, 2008, 00:30
Default Re: error in AMG solver
  #8
Ant
Guest
 
Posts: n/a
Hi,

Send me a message with more details about ur setup.. My Masters thesis was on solid settling behaviour of clarifiers!
  Reply With Quote

Old   April 8, 2008, 00:33
Default Re: error in AMG solver
  #9
Ant
Guest
 
Posts: n/a
Sudhir,

Your case is much more complicated that it seems. Ur actually simulating natural convection. Did you calculate what the Raleigh number is for your case?

Your mesh needs to be really fine near the walls to capture the sharp temperature gradients.

Send me an email and I would try and get back to you when I have some time.
  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
FSI Solver error CC CFX 3 October 3, 2008 11:06
Solver Error eros CFX 1 July 4, 2007 08:03
cfx 5.7 solver error hazri CFX 1 March 2, 2005 05:14
CFX 5.7 solver error Neser CFX 9 March 1, 2005 11:59
Error in AMG Solver: help please madasu FLUENT 1 August 16, 2002 07:14


All times are GMT -4. The time now is 20:57.