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

Conjugate Heat Transfer in CFX

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 21, 2010, 19:28
Default Conjugate Heat Transfer in CFX
  #1
New Member
 
Maher Al-Dojayli
Join Date: Mar 2010
Posts: 3
Rep Power: 7
Maher Al-Dojayli is on a distinguished road
Hello All,

I am modeling a simple problem which is conjugate heat transfer in ANSYS CFX. It is a heat sink fin where there is a forced convection.

I run the model and it did converge and the solution made sense. However, it did solve when the mesh of the fin (solid) is coarse, one element per thinkness of the fin. I was able to refine the air medium mesh but as soon as refine the solid mesh ( no matter at what level), ANSYS fails to solve. It starts solving then stops with the following error:

-----------------------------------------------------------
ERROR #001100279 has occurred in subroutine ErrAction.
Message:
SYMASS_CS_ELIM : The solver ran out of temporary space while building a linked list for a domain.


Details of error:-
----------------
Error detected by routine POPDIR
CRESLT = ILEG
-----------------------------------------------------------

I have read some threads about this matter. Nothing really helped.
I put it as Double Precision
I put the memory allocation factor as 1.5

Nothing works. I do not think they matter since the memory was enough for the refine mesh of the air medium which much more than the solid.

Any help in this regard is very much appreciated

Maher

Last edited by Maher Al-Dojayli; March 22, 2010 at 11:19.
Maher Al-Dojayli is offline   Reply With Quote

Old   March 21, 2010, 19:50
Default Conjugate Heat Transfer in CFX
  #2
New Member
 
Maher Al-Dojayli
Join Date: Mar 2010
Posts: 3
Rep Power: 7
Maher Al-Dojayli is on a distinguished road
Dear all,

Never mind of the blog. I have solved it.

It was the topology estimate factor as indicated in the error file. I have changed it to a factor of 1.2. This can be done from the CFX-Solver Expert Control Parameters.

Thank you all anyways

Maher

Last edited by Maher Al-Dojayli; March 22, 2010 at 11:19.
Maher Al-Dojayli is offline   Reply With Quote

Old   August 6, 2010, 13:24
Default
  #3
Senior Member
 
Join Date: Feb 2010
Posts: 145
Rep Power: 8
Jade M is on a distinguished road
Please see below some more detailed information from ANSYS Tech Support.

A change in the CFX solver from V 11.0 to V 12.0 has caused CFX to underestimate memory for certain types of problems. Memory usage almost always scales with the number of elements in a problem. In Pre, in the Outline, under Simulation, Flow Analysis 1 and Solver, right click on Expert Parameters and click Edit. Click on tab Convergence Control and, under Memory Control, check topology estimate factor and set the value greater than 1.0. This parameter is a multiplier that scales the memory allocated for topology. Recommended values are 1.2 to 1.4. The memory allocation depends on several factors, which are mesh size, physics, number of nodes at mesh interfaces or periodic planes, and partitioning or complexity of the geometry. Failure corresponds with the calculation where the first memory overrun occurs.
Jade M is offline   Reply With Quote

Old   August 6, 2010, 17:23
Default
  #4
New Member
 
Maher Al-Dojayli
Join Date: Mar 2010
Posts: 3
Rep Power: 7
Maher Al-Dojayli is on a distinguished road
Thank you Jade!

Yes, that's what I did back then. It does suggest doing so. However, I did not know the reason behind it. Now, I know.

Thank you again for the clarification

Maher
Maher Al-Dojayli is offline   Reply With Quote

Old   August 6, 2010, 17:25
Default
  #5
Senior Member
 
Join Date: Feb 2010
Posts: 145
Rep Power: 8
Jade M is on a distinguished road
You're most welcome, Maher!

I like spreading the knowledge, but also documenting these sorts of things. I have my own "best practices" and random notes but this'll be a great resource if I ever lose or don't have access to them.

Take care!
Jade M is offline   Reply With Quote

Old   November 1, 2011, 22:06
Default
  #6
New Member
 
Join Date: Nov 2011
Posts: 1
Rep Power: 0
bubupo is on a distinguished road
I have find the option under Solver , right click then add expert parameters. After setting up, it worked.
bubupo is offline   Reply With Quote

Reply

Tags
cfx, conjugate heat transfer, error #001100279

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
Convective / Conductive Heat Transfer in Hypersonic flows enigma Main CFD Forum 2 November 1, 2009 23:53
Conjugate heat transfer problem hvem10 FLUENT 2 October 29, 2009 18:31
CFX Heat Transfer RJamison CFX 0 July 24, 2008 12:11
conjugate heat transfer in circular channel src FLUENT 1 August 6, 2004 07:13
Conjugate heat transfer (vs) periodic boundary mp FLUENT 1 January 13, 2003 02:38


All times are GMT -4. The time now is 15:36.