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

Divergence Problem Conjugated Heat Transfer

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

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   November 27, 2017, 07:08
Default
  #21
New Member
 
Christoph Hahn
Join Date: Nov 2017
Posts: 14
Rep Power: 3
Christoph.Ha is on a distinguished road
The think is, i also want to get the surface temperatures of the solid housing. So it would be necessary to make a simulation with fluid and solid part.
Christoph.Ha is offline   Reply With Quote

Old   November 27, 2017, 07:54
Default
  #22
New Member
 
Moritz Kuhn
Join Date: Apr 2010
Location: Dresden
Posts: 26
Rep Power: 10
MKuhn is on a distinguished road
In my opinion you will get nearly the same results without solid mesh and wall thickness+shell conduction instead. Which is the thermal condition on your outer wall? (Heat flux, fixed temperature or convection?)
MKuhn is offline   Reply With Quote

Old   November 27, 2017, 09:38
Default
  #23
New Member
 
Christoph Hahn
Join Date: Nov 2017
Posts: 14
Rep Power: 3
Christoph.Ha is on a distinguished road
Its a heat flux, but coupled with a heat generation rate inside an electrical componend which is coupled to the wall. In an later step i want to model this electircal componend also, therefore i think i need that wall physically?
Christoph.Ha is offline   Reply With Quote

Old   November 27, 2017, 10:36
Default
  #24
New Member
 
Moritz Kuhn
Join Date: Apr 2010
Location: Dresden
Posts: 26
Rep Power: 10
MKuhn is on a distinguished road
You can also impose a heat load (Heat Generation Rate in w/m) to a shell conduction layer. Please refer to here and here.
MKuhn is offline   Reply With Quote

Old   November 27, 2017, 20:54
Default
  #25
Senior Member
 
Alexander
Join Date: Apr 2013
Posts: 387
Rep Power: 10
AlexanderZ is on a distinguished road
Quote:
Originally Posted by Christoph.Ha View Post
Hello,

i have some news. Today i tested an setup without the solid wall, so just the fluid domain. That converged very well and max. Velocitys are <10m/s (with an inlet Velocity of 5m/s). So i think there must be something wrong with the interface.
During initialization i get following info: "Info: Interface zones overlap for mesh interface contact_region.
This could adversely affect your solution."
After some research i found out, that the walls of both domains have some issus with the contact definition. But im not aware of how i could solve that issue, does anybody of you guys can tell me how to fix it?

Thanks in advance,
Christoph

EDIT: Mesh -> Contacts -> Contact Region shows Contact: 686 Faces, Target: 687 Faces. Scoping Method is Geometry Selection.
I think, for your case you do not need contacts.
Delete them before loading mesh into fluent. In case you are using ansys mesher go to mesh -> contacts -> delete contacts.

Than load mesh into fluent, define materials for solid and fluid parts.
use
Code:
mesh m-z s-i-b
This will create shadows between solids, in case you have more than one.

Best regards
AlexanderZ is online now   Reply With Quote

Old   November 29, 2017, 07:32
Default
  #26
New Member
 
Ovid
Join Date: Oct 2016
Location: Spain
Posts: 28
Rep Power: 4
Fole is on a distinguished road
If I were you:

1) Change to kwSST standard (no transition). Because y+=1 is a must in that model.
2) Check y+ and BL resolution. If after reducing speed your model converged, maybe it is the cause.
3) In my experience, inflation on complex geometries, I limit the transition ratio even more (limiting the height), and then adaptive mesh refinement during solution. ICEM CFD is another solution, I am on the way.
Fole is offline   Reply With Quote

Old   December 5, 2017, 02:43
Default
  #27
New Member
 
Christoph Hahn
Join Date: Nov 2017
Posts: 14
Rep Power: 3
Christoph.Ha is on a distinguished road
Hello Guys,

i found the problem!
It was a problem with the interface between the fluid and the solid wall!
I solved it with a mapped (+coupled) interface between those domains. No it converges very well with k-e-model and energy equation!

Thank you all very much, i still learned a lot about troubleshooting with fluent divergence!

Best Regards,
Christoph
Christoph.Ha is offline   Reply With Quote

Old   December 5, 2017, 11:46
Default
  #28
New Member
 
Moritz Kuhn
Join Date: Apr 2010
Location: Dresden
Posts: 26
Rep Power: 10
MKuhn is on a distinguished road
Hi Christoph,

thanks for your reply, fine that its works now

Moritz
MKuhn is offline   Reply With Quote

Reply

Tags
amg solver, convergence, divergence, fluent, omega

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 conjugate heat transfer problem eling FLUENT 9 October 21, 2017 11:10
CFD analysis of a heat transfer problem vinitraj3 Main CFD Forum 0 May 2, 2015 06:35
heat transfer validation problem messbalint CFX 4 March 31, 2012 17:14
Heat Flux at wall in a conjugate heat transfer problem Chander CFX 2 July 9, 2011 23:22
regarding B.C. of Heat transfer problem Manoj Padmakarrao Raut Siemens 0 March 17, 2005 01:01


All times are GMT -4. The time now is 00:56.