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

Ask for help: CFX solution error

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   December 6, 2021, 01:35
Default Ask for help: CFX solution error
  #1
New Member
 
Han changho
Join Date: Dec 2021
Posts: 1
Rep Power: 0
novice_han is on a distinguished road
Hello, I am a student studying CFX.

I am doing CFD to check the heat exchange state of the fin-and-tube heat exchanger, but an error occurs and I ask this question.

The error is, after setup, the solution does not work at all, and the message "Update failed for the Solution component in Fluid Flow (CFX). The solver failed with a non-zero exit code of : 2" is displayed.

I am attaching my CFX capture file, so please advise.

thank you.


---------------------------------------------------------------------------
| |
| Partitioning |
| |
+--------------------------------------------------------------------+




+--------------------------------------------------------------------+
| |
| ANSYS(R) CFX(R) Partitioner |
| |
| 2020 R2 |
| Build 20.2 2020-05-29T15:06:09.465000 |
| Fri May 29 17:25:52 GMTDT 2020 |
| |
| Executable Attributes |
| |
| double-64bit-int32-archfort-optimised-std-lcomp |
| |
| (C) 1996-2020 ANSYS, Inc. |
| |
| All rights reserved. Unauthorized use, distribution or duplication |
| is prohibited. This product is subject to U.S. laws governing |
| export and re-export. For full Legal Notice, see documentation. |
+--------------------------------------------------------------------+




+--------------------------------------------------------------------+
| Job Information at Start of Run |
+--------------------------------------------------------------------+

Run mode: partitioning run

Host computer: DESKTOP-HGJOG82 (PID:9056)

Job started: Mon Dec 6 15:11:01 2021

+--------------------------------------------------------------------+
| License Information |
+--------------------------------------------------------------------+

License Cap: ANSYS CFX Solver (> 512K Nodes)
License Cap: Parallel
License ID: DESKTOP-QE253AB-SYSTEM-4940-452479


+--------------------------------------------------------------------+
| Memory Allocated for Run (Actual usage may be less) |
+--------------------------------------------------------------------+

| Real | Integer | Character | Logical | Double
----------+------------+------------+-----------+----------+----------
Mwords | 302.86 | 604.04 | 11.33 | 0.12 | 0.00
Mbytes | 2310.64 | 2304.24 | 10.81 | 0.46 | 0.00
----------+------------+------------+-----------+----------+----------


+--------------------------------------------------------------------+
| Host Memory Information (Mbytes) |
+--------------------------------------------------------------------+
| Host | System | Allocated | % |
+-------------------------+----------------+----------------+--------+
| DESKTOP-HGJOG82 | 65369.57 | 4626.15 | 7.08 |
+-------------------------+----------------+----------------+--------+

+--------------------------------------------------------------------+
| The MeTiS partitioning method allocates additional memory. |
| Total memory usage will therefore exceed the values shown above. |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| Topology Simplification |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| ****** Warning ****** |
| |
| Topology simplification is activated with the following |
| restrictions: |
| |
| - Mesh regions referenced only within User Fortran and NOT |
| in the command file will cause the solver to stop. |
| - The solver will stop during any "Edit Run in Progress" step |
| if new 2D regions are referenced. |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| *** INSUFFICIENT CATALOGUE SIZE *** |
| |
| ACTION REQUIRED : Increase the file catalogue size. |
| |
| If the situation persists please contact the CFX Customer Helpline |
| giving the following details:- |
| Current catalogue size : 230867 |
+--------------------------------------------------------------------+


Details of error:-
----------------
Error detected by routine MAKLNK
COLDNM = ../../ZN4/BELG658 CNEWNM = BELG2
CRESLT = FCAT

Current Directory : /FLOW/MESH/TSTEP0/CLOOP0/ZIF2/BELGP552

+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| The ANSYS CFX partitioner exited with return code 1. |
+--------------------------------------------------------------------+


+--------------------------------------------------------------------+
| For CFX runs launched from Workbench, the final locations of |
| directories and files generated may differ from those shown. |
+--------------------------------------------------------------------+


This run of the ANSYS CFX Solver has finished.
Attached Images
File Type: jpg CFX_1_model.jpg (83.4 KB, 11 views)
File Type: jpg CFX_2_mesh.jpg (83.9 KB, 10 views)
File Type: jpg CFX_3_setup.jpg (66.9 KB, 10 views)
File Type: jpg CFX_4_solution_error_message.jpg (29.7 KB, 8 views)
novice_han is offline   Reply With Quote

Old   December 6, 2021, 03:16
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
The snippet from the output file is the one with the information in it. Workbench is useless for debugging.

(Oops, my original post was wrong. Here is a corrected one )

Your memory is OK, it is failing to get the catalog size right. This is usually caused by models with very complex topology, with lots of surfaces and faces.

The best way to fix this problem is to load you mesh in a mesh editing program (eg ICEM) and edit your mesh so the hundreds of surfaces are merged into the handful you actually need. So by default every surface is its own face - when there are too many you get catalog size errors.

An alternate way is to use a different partitioning algorithm (eg recursive bisection). It might not work, but if it does it is a quick and easy fix.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   December 6, 2021, 06:08
Default
  #3
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,827
Rep Power: 27
Gert-Jan will become famous soon enough
You can also try to increase the memory allocated by CFX, or specifically increase the catalogue size.
You can find these in these "Define Run"-window of the Solver manager by ticking "Show Advanced Control"
Then under Solver > Solver Memory


If this does not help, and you the MAKLNK error keeps on appearing, then your setup is incorrect.
Gert-Jan is offline   Reply With Quote

Old   December 6, 2021, 07:10
Default
  #4
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,827
Rep Power: 27
Gert-Jan will become famous soon enough
Correction: your error occurs in the partitioning stage.
So, in the Advanced Control menu go to Partioner > Detailed Memory Overrides
And change settings here...

It the error persists, you could try a different partitioning method that requires less memory, like recursive bisection. Alternatively, use a directional method. I would use the z-direction in your case.
Gert-Jan is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[swak4Foam] GroovyBC the dynamic cousin of funkySetFields that lives on the suburb of the mesh gschaider OpenFOAM Community Contributions 300 October 29, 2014 18:00
OpenFOAM without MPI kokizzu OpenFOAM Installation 4 May 26, 2014 09:17
Compiling dynamicTopoFvMesh for OpenFOAM 2.1.x Saxwax OpenFOAM Installation 25 November 29, 2013 05:34
user subroutine error CFDUSER CFX 2 December 9, 2006 06:31
Could anybody help me see this error and give help liugx212 OpenFOAM Running, Solving & CFD 3 January 4, 2006 18:07


All times are GMT -4. The time now is 08:54.