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

Joule heating convergence problem

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 16, 2010, 09:46
Default Joule heating convergence problem
  #1
New Member
 
Shahid Parvez
Join Date: Jul 2009
Location: Pakistan
Posts: 25
Rep Power: 7
shahpar73 is on a distinguished road
Hi
I am simulating Joule heating. There are two domains, one is solid electrode (copper) and other is Fluid (Argon with temperature dependent electrical conductivity and others).
I apply current at the top of the solid electrode as electric field flux in. Simulation converges at a current flux of 25 [A m-2] but when I change it to actual value of 25000000 [A m-2] the solution diverges after 4 iterations. Error message is bellow:

+--------------------------------------------------------------------+
| ****** Notice ******
| While evaluating Static Enthalpy,
| Static Pressure
| went outside of its lower limit. Its minimum value was
| -2.4670E+11. The bounds error was handled by clipping.
| If this situation persists, consider increasing the table range.
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| ERROR #004100018 has occurred in subroutine FINMES.
| Message:
| Fatal overflow in linear solver.
+--------------------------------------------------------------------+

Help please...

Regards
shahpar73 is offline   Reply With Quote

Old   January 16, 2010, 17:03
Default
  #2
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
Only guess, the problem is with the fineness of your mesh...
Attesz is offline   Reply With Quote

Old   January 16, 2010, 17:09
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Looks like a simple divergence to me. Fixing it could mean many things. Also there is a power 1e6 difference between your two tests - that probably means they have very little in relation to each other, just as a Re=1 flow looks nothing like a Re=1e6 flow. Try some intermediate fluxes.

You will almost certainly need a smaller timestep for the higher heating rate one. Also local timescale factor to start things off might help.

Also consider simplifying the problem. Start with the simplest physics possible and get that to converge. Add the physics one at a time until you have all the physics working.

Also have a look here:
http://www.cfd-online.com/Wiki/Ansys...gence_criteria
ghorrocks is offline   Reply With Quote

Old   January 17, 2010, 00:02
Default
  #4
New Member
 
Shahid Parvez
Join Date: Jul 2009
Location: Pakistan
Posts: 25
Rep Power: 7
shahpar73 is on a distinguished road
Thanks for the reply.
Can you please comment on the error message bellow? what this mean? how to increase the table range? and will it help in convergence?
+--------------------------------------------------------------------+
| ****** Notice ******
| While evaluating Total Enthalpy,
| Static Pressure
| went outside of its upper limit. Its maximum value was
| 6.3200E+10. The bounds error was handled by clipping.
| If this situation persists, consider increasing the table range.
+--------------------------------------------------------------------+
shahpar73 is offline   Reply With Quote

Old   January 17, 2010, 06:25
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
As I said, your simulation has diverged. The message says the maximum pressure was 6e10. This is almost certainly physically impossible so is the sign of a rapidly diverging simulation. Only increase the table range if this pressure is likely to be correct. If it is not correct then fix the divergence and the problem will be fixed.
ghorrocks is offline   Reply With Quote

Old   January 17, 2010, 09:30
Default
  #6
Senior Member
 
ckleanth's Avatar
 
George
Join Date: Mar 2009
Location: Birmingham, UK
Posts: 257
Rep Power: 9
ckleanth is on a distinguished road
assuming you are modeling ionisation of argon, the plasma core can reach extreme temperatures in excess of 15K [K] hense the divergence.

if you have modified the fluid properties taking in to account the range of temperatures refine your mesh, use small timesteps and use underelax on
enthalpy, entropy, conelec and jcur.
__________________
Top 4 tips
1. Knowledge is everything and Ignorance is dangerous.
2. Understand your limitations and try to eliminate them.
3. Get yerself a bike and hoon the chuffer. You will soon learn why dogs like to hang their heads out the car window.
4. Please before asking any questions on how to run simulations in CFX, go though all the tutorials
ckleanth is offline   Reply With Quote

Old   January 17, 2010, 09:34
Default
  #7
New Member
 
Shahid Parvez
Join Date: Jul 2009
Location: Pakistan
Posts: 25
Rep Power: 7
shahpar73 is on a distinguished road
What about the ramp loading concept? What if I apply 25 in first iteration then 25e1, 25e2.....and 25e6 in the succeeding iterations? will it help in convergence?
shahpar73 is offline   Reply With Quote

Old   January 17, 2010, 09:44
Default
  #8
Senior Member
 
ckleanth's Avatar
 
George
Join Date: Mar 2009
Location: Birmingham, UK
Posts: 257
Rep Power: 9
ckleanth is on a distinguished road
if the divergence is because of the high temperature thus your energy equation falls apart, do you think that ramping the flux will help? the emag module is also very demanding on the mesh resolution so sort your physics and mesh first, and as glenn said, get simplest physics possible to converge and add more complexity bit by bit
__________________
Top 4 tips
1. Knowledge is everything and Ignorance is dangerous.
2. Understand your limitations and try to eliminate them.
3. Get yerself a bike and hoon the chuffer. You will soon learn why dogs like to hang their heads out the car window.
4. Please before asking any questions on how to run simulations in CFX, go though all the tutorials
ckleanth is offline   Reply With Quote

Old   January 19, 2010, 00:06
Default
  #9
New Member
 
Shahid Parvez
Join Date: Jul 2009
Location: Pakistan
Posts: 25
Rep Power: 7
shahpar73 is on a distinguished road
Dear Goerge
Thanks for the comments. Yes you right, its about the ionization of Argon.
Can you please also comment on how to set under-relaxation(s) you mentioned in your post?
shahpar73 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
convergence problem commonyue Main CFD Forum 1 December 1, 2009 04:54
Convergence of CFX field in FSI analysis nasdak CFX 2 June 29, 2009 01:17
convergence problem alexandre FLUENT 2 June 14, 2007 14:31
3D Fluid Flow Convergence problem Emily FLUENT 2 March 21, 2007 23:18
Non Convergence of 3D Heat transfer cfd problem Balraj Main CFD Forum 3 December 9, 2004 01:24


All times are GMT -4. The time now is 08:48.