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

Unexplained Error during Solver Runs

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 1, 2012, 21:16
Question Unexplained Error during Solver Runs
  #1
cfb
New Member
 
Fahad Bashir
Join Date: Nov 2012
Posts: 4
Rep Power: 4
cfb is on a distinguished road
I'm trying to simulate bubble based flow in columns using CFX. I've been trying to run my simulations but I keep receiving the same error over and over again related to a missing variable that I have been unable to track down. More specifically the error is:

Error in subroutine FNDVAR :
Error finding variable TED_FL2
GETVAR originally called by subroutine cal_COALESCE

I've tried looking through help files, tutorials, online forums but I've not been able to encounter this error or any reasons for it elsewhere. If anyone has any ideas or has experienced this problem before, I would love to hear from them.

The original solver output is pasted below for reference. Thank you for your time and cooperation.


CFD Solver started: Fri Nov 02 06:02:47 2012


+--------------------------------------------------------------------+
| Convergence History |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| Writing transient file 0_full.trn |
| Name : Transient Results 1 |
| Type : Standard |
| Option : Every Timestep |
+--------------------------------------------------------------------+


================================================== ====================
| Timestepping Information |
----------------------------------------------------------------------
| Timestep | RMS Courant Number | Max Courant Number |
+----------------------+----------------------+----------------------+
| 1.0000E-01 | 0.00 | 0.00 |
----------------------------------------------------------------------

================================================== ====================
TIME STEP = 1 SIMULATION TIME = 1.0000E-01 CPU SECONDS = 1.042E+01
----------------------------------------------------------------------
COEFFICIENT LOOP ITERATION = 1 CPU SECONDS = 1.042E+01
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| U-Mom-Fluid 1 | 0.00 | 1.2E-04 | 1.2E-03 | 1.8E+00 F |
| V-Mom-Fluid 1 | 0.00 | 6.3E-01 | 7.1E-01 | 1.2E-04 OK|
| W-Mom-Fluid 1 | 0.00 | 1.3E-04 | 1.2E-03 | 1.8E+00 F |
| U-Mom-Air | 0.00 | 1.3E-19 | 1.5E-18 | 3.9E+07 F |
| V-Mom-Air | 0.00 | 1.2E-19 | 1.1E-18 | 2.0E+09 F |
| W-Mom-Air | 0.00 | 1.3E-19 | 1.0E-18 | 3.8E+07 F |
| P-Vol | 0.00 | 3.2E-07 | 7.7E-06 | 42.4 2.0E+00 F |
+----------------------+------+---------+---------+------------------+
| Mass-Fluid 1 | 0.00 | 2.5E-02 | 8.8E-01 | 5.4 8.4E-03 OK|
| Mass-Air | 0.00 | 2.7E-02 | 9.7E-01 | 5.4 7.3E-03 OK|
+----------------------+------+---------+---------+------------------+
----------------------------------
Error in subroutine FNDVAR :
Error finding variable TED_FL2
GETVAR originally called by subroutine cal_COALESCE

+--------------------------------------------------------------------+
| Writing crash recovery file |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Stopped in routine GV_ERROR |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| The ANSYS CFX solver exited with return code 1. No results file |
| has been created. |
+--------------------------------------------------------------------+

End of solution stage.

+--------------------------------------------------------------------+
| The following transient and backup files written by the ANSYS CFX |
| solver have been saved in the directory G:\Bubbles\B&C\bub__004: |
| |
| 0_full.trn |
+--------------------------------------------------------------------+


+--------------------------------------------------------------------+
| Warning! |
| |
| The ANSYS CFX Solver has written a crash recovery file. This file |
| has been saved as G:\Bubbles\B&C\bub__004.res.err and may be an |
| aid to diagnosing the problem or restarting the run. More details |
| should be available in the solver output section of the output |
| file. |
+--------------------------------------------------------------------+


+--------------------------------------------------------------------+
| The following user files have been saved in the directory |
| G:\Bubbles\B&C\bub__004: |
| |
| mon |
+--------------------------------------------------------------------+


This run of the ANSYS CFX Solver has finished.
cfb is offline   Reply With Quote

Old   November 3, 2012, 05:42
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You have missed a necessary parameter in your set up. My guess is it is something to do with turbulence dissipation. So is your turbulent conditions properly specified? Or some interaction between your bubble coalescence model and turbulence?
ghorrocks is online now   Reply With Quote

Old   November 3, 2012, 06:47
Default
  #3
cfb
New Member
 
Fahad Bashir
Join Date: Nov 2012
Posts: 4
Rep Power: 4
cfb is on a distinguished road
Thank you for your reply. I'm using the LES WALE turbulence model but it requires nothing else to be specified in terms of dissipation (as far as my knowledge on the issue goes). Do you have any idea if some coefficient or other such parameter needs to be inserted with LES WALE?
There is another interesting observation I have with regards to this problem. As soon as I turn off the coalescence model, the error repeats for the breakup model. If I turn that off as well, the entire simulation proceeds smoothly. I've checked both these areas for turbulence modelling but have found nothing to go with. Any other ideas
cfb is offline   Reply With Quote

Old   November 3, 2012, 15:21
Default
  #4
New Member
 
Join Date: Dec 2009
Posts: 29
Rep Power: 7
cfdgremlin is on a distinguished road
The solver is looking for Turbulence Eddy Dissipation in one of the phases but can't find it. Check your turbulence models for each phase.

cal_COALESCE seems to me to be related to MUSIG, so are you trying to run inhomogeneous MUSIG with LES?

CG
cfdgremlin is offline   Reply With Quote

Old   November 3, 2012, 17:21
Lightbulb @cfdgremlin
  #5
cfb
New Member
 
Fahad Bashir
Join Date: Nov 2012
Posts: 4
Rep Power: 4
cfb is on a distinguished road
My turbulence model for water is LES WALE while it is Dispersed Phase Zero Equation for air (bubbles) but I've not specified any parameters for any model at all.
Also, I'm trying to run LES with homogenous MUSIG right now. Plus, where could I get guidelines for Eddy Viscosity Prandtl Number and LES WALE Model Constant?
Thank you for the help cfdgremlin and ghorrocks.
cfb is offline   Reply With Quote

Old   November 3, 2012, 17:39
Default
  #6
cfb
New Member
 
Fahad Bashir
Join Date: Nov 2012
Posts: 4
Rep Power: 4
cfb is on a distinguished road
@cfdgremlin
--> I've used a LES WALE Model Constant of 0.325 based on recommendations from:
https://www.sharcnet.ca/Software/Flu.../th/node95.htm

I run the Solver after that and it started iterating though I'm not done with the complete iteration as yet. This seems to have relieved the issue but I would really appreciate if you could please comment on the use of this constant value given water bubble flow in a homogeneous MUSIG regime. Thank you.
cfb is offline   Reply With Quote

Old   November 9, 2012, 16:42
Default
  #7
New Member
 
Join Date: Dec 2009
Posts: 29
Rep Power: 7
cfdgremlin is on a distinguished road
Hi cfb,

sorry, but I'm not an LES or MUSIG expert so I can't offer any advice on the parameters. However, I'm surprised you managed to get the case going by simply modifying/adding the constant, because as Glenn pointed out the initial error is due to a problem with general physics setup.

All the best,

CG
cfdgremlin is offline   Reply With Quote

Reply

Tags
cal_coalesce, error, findvar, getvar, ted_fl2

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
Quarter Burner mesh with periosic condition SamCanuck FLUENT 2 August 31, 2011 11:34
Solver Error before it even Runs trex930 OpenFOAM Running, Solving & CFD 10 April 25, 2011 23:23
Working directory via command line Luiz CFX 4 March 6, 2011 21:02
why the solver reject it? Anyone with experience? bearcat CFX 6 April 28, 2008 14:08
Error during Solver cfd guy CFX 4 May 8, 2001 06:04


All times are GMT -4. The time now is 03:07.