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

If anyone came across this error, please help!!!!

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

Like Tree1Likes
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Display Modes
Old   August 12, 2009, 03:46
Exclamation If anyone came across this error, please help!!!!
  #1
Member
 
geothokar's Avatar
 
George Thomas
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 59
Rep Power: 8
geothokar is on a distinguished road
Hi,

I was simulating an IC engine model. I successfully did the same simulation with the same set ups (in fact the same file) without any error at an earlier time.

Recently I was trying to run it again, and every time I am getting this error.

ERROR #001100279 has occurred in subroutine ErrAction.
Message:
c_fpx_handler: Floating point exception: Overflow

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

Current Directory : /FLOW/NAMEMAP

An error has occurred in cfx5solve:

The ANSYS CFX solver exited with return code 1. No results file
has been created.

If anyone ever came across similar error, please help me how to solve this, or help me what this error means.
__________________
Cheers,

George

"The fact that I can plant a seed and it becomes a flower, share a bit of knowledge and it becomes another's, smile at someone and receive a smile in return, are to me continual spiritual exercises"Leo.F. Buscaglia
geothokar is offline   Reply With Quote

Old   August 12, 2009, 07:11
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,937
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Floating point exception: overflow usually means your simulation has diverged big-time. You need to make the simulation more stable. It can also mean you snuck a divide by zero in there but generally it is caused by divergence.

Glenn Horrocks
ghorrocks is online now   Reply With Quote

Old   August 13, 2009, 05:28
Default reply
  #3
New Member
 
dss
Join Date: Jul 2009
Posts: 25
Rep Power: 8
flyingd is on a distinguished road
please check your model and mesh carefully!!!
flyingd is offline   Reply With Quote

Old   August 13, 2009, 21:16
Default
  #4
Member
 
geothokar's Avatar
 
George Thomas
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 59
Rep Power: 8
geothokar is on a distinguished road
I think remeshing the model and reducing the time step can solve this issue to some extend. But, it there any other ways to try to increase stability?
__________________
Cheers,

George

"The fact that I can plant a seed and it becomes a flower, share a bit of knowledge and it becomes another's, smile at someone and receive a smile in return, are to me continual spiritual exercises"Leo.F. Buscaglia
geothokar is offline   Reply With Quote

Old   August 13, 2009, 23:00
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,937
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Things which will improve stability and accuracy are to improve mesh quality, reduce timestep size, swap to double precision, a better initial guess and tighter convergence.

Things which will improve stability but reduce accuracy are use 1st order discretisation for spatial and time discretisation and under-relaxation.

Definitely try the first options as they can be safely done without compromising accuracy before trying upwinding or under-relaxation which will reduce accuracy.

Glenn Horrocks
ghorrocks is online now   Reply With Quote

Old   August 13, 2009, 23:01
Default reply
  #6
New Member
 
dss
Join Date: Jul 2009
Posts: 25
Rep Power: 8
flyingd is on a distinguished road
Hi:
check the mesh quality, angles!!!
angles>18
quality>0.25
It is well mesh.
flyingd is offline   Reply With Quote

Old   August 14, 2009, 09:25
Default
  #7
Senior Member
 
Join Date: Jul 2009
Posts: 211
Rep Power: 9
kingjewel1 is on a distinguished road
Quote:
Originally Posted by flyingd View Post
Hi:
check the mesh quality, angles!!!
angles>18
quality>0.25
It is well mesh.
What do you find is the best tool to check mesh quality in CFX ?
kingjewel1 is offline   Reply With Quote

Old   August 14, 2009, 20:45
Default
  #8
Member
 
geothokar's Avatar
 
George Thomas
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 59
Rep Power: 8
geothokar is on a distinguished road
I presume what flyingd meant by 'to check the mesh quality', is to use ICEM to check the mesh.

Could you clarify it flyingd.
__________________
Cheers,

George

"The fact that I can plant a seed and it becomes a flower, share a bit of knowledge and it becomes another's, smile at someone and receive a smile in return, are to me continual spiritual exercises"Leo.F. Buscaglia
geothokar is offline   Reply With Quote

Old   August 14, 2009, 21:02
Default reply
  #9
New Member
 
dss
Join Date: Jul 2009
Posts: 25
Rep Power: 8
flyingd is on a distinguished road
Yes ,using icme check your mesh quality. If it is not well.
The soft does't calculate.
flyingd is offline   Reply With Quote

Old   August 14, 2009, 21:49
Default
  #10
Member
 
geothokar's Avatar
 
George Thomas
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 59
Rep Power: 8
geothokar is on a distinguished road
Thanks flyingd for the reply.

Anyone has any idea about the following error?

ERROR #004100008 has occurred in subroutine FINDL.
Message:
Insufficient space for array LNOD.
__________________
Cheers,

George

"The fact that I can plant a seed and it becomes a flower, share a bit of knowledge and it becomes another's, smile at someone and receive a smile in return, are to me continual spiritual exercises"Leo.F. Buscaglia
geothokar is offline   Reply With Quote

Old   August 16, 2009, 02:32
Default
  #11
New Member
 
Basavaraj
Join Date: Aug 2009
Posts: 4
Rep Power: 8
basavaraj.pyati is on a distinguished road
Quote:
Originally Posted by geothokar View Post
Hi,

I was simulating an IC engine model. I successfully did the same simulation with the same set ups (in fact the same file) without any error at an earlier time.

Recently I was trying to run it again, and every time I am getting this error.

ERROR #001100279 has occurred in subroutine ErrAction.
Message:
c_fpx_handler: Floating point exception: Overflow

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

Current Directory : /FLOW/NAMEMAP

An error has occurred in cfx5solve:

The ANSYS CFX solver exited with return code 1. No results file
has been created.

If anyone ever came across similar error, please help me how to solve this, or help me what this error means.
The reasons for getting floating point error are
1) You may not initialized your solution with proper values(here you can initialise your solutions with previous results values)

2) Time step values(If u r using auto time step,plese use phsical time step and start with smaller value(smaller than auto time step value)).

You asked one more query on memory space ,Since you are solving for IC engine your node count may be very high,so keep sufficiently large space in your working directory (min of 5 to 6 GB)
basavaraj.pyati is offline   Reply With Quote

Old   August 1, 2011, 10:05
Default
  #12
New Member
 
Join Date: May 2011
Location: Duisburg, Germany
Posts: 5
Rep Power: 6
ovechkin is on a distinguished road
Is this error (c_fpx_handler: Floating point exception: Overflow) related to the applied turbulence model?

my setup works fine when i calculate using SST model but solver exits when using k-epsilon EARSM model.

i already tried reducing physical timestep size but without success. what other reasons could cause this problem?

regards
ovechkin is offline   Reply With Quote

Old   August 1, 2011, 18:29
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,937
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
My first post in this thread explains the error: Floating point exceptions are the result of a major divergence in the numerics. A large range of things can cause the divergence, it includes turbulence models, mesh quality, time step size, physics selection and many others.

You need to improve the stability of the numerics. Assuming you have the basics under control often the most effective way to do this is to improve the mesh quality.
ghorrocks is online now   Reply With Quote

Old   November 16, 2011, 14:18
Default
  #14
Member
 
Julian Krick
Join Date: May 2009
Location: Guelph
Posts: 88
Rep Power: 8
Julian K. is on a distinguished road
Hi!

I get the same error, when the solver tries to write the backup file:
Code:
 +--------------------------------------------------------------------+
 | Writing backup file 740_full.bak                                   |
 |   Name   : Backup Results 1                                        |
 |   Type   : Standard                                                |
 |   Option : Timestep Interval                                       |
 +--------------------------------------------------------------------+
 
 +--------------------------------------------------------------------+
 | ERROR #001100279 has occurred in subroutine ErrAction.             |
 | Message:                                                           |
 | c_fpx_handler: Floating point exception: Overflow                  |
 |                                                                    |
 |                                                                    |
 |                                                                    |
 |                                                                    |
 |                                                                    |
 +--------------------------------------------------------------------+
 
 +--------------------------------------------------------------------+
 | ERROR #001100279 has occurred in subroutine ErrAction.             |
 | Message:                                                           |
 | Stopped in routine FPX: c_fpx_handler                              |
 |                                                                    |
 |                                                                    |
 |                                                                    |
 |                                                                    |
 |                                                                    |
 +--------------------------------------------------------------------+

 +--------------------------------------------------------------------+
 |                An error has occurred in cfx5solve:                 |
 |                                                                    |
 | The ANSYS CFX solver exited with return code 1.   No results file  |
 | has been created.                                                  |
 +--------------------------------------------------------------------+
ICEM output for mesh quality is:
Code:
Min = 1.87501e-07, max = 1, mean = 0.976192191698
194306 elements with the "Quality" diagnostic
Histogram of Quality values
0.95 -> 1.0 : 185006 (95.214%)
0.9 -> 0.95 : 3661 (1.884%)
0.85 -> 0.9 : 2261 (1.164%)
0.8 -> 0.85 : 1632 (0.840%)
0.75 -> 0.8 : 1125 (0.579%)
0.7 -> 0.75 : 525 (0.270%)
0.65 -> 0.7 : 15 (0.008%)
0.6 -> 0.65 : 21 (0.011%)
0.55 -> 0.6 : 11 (0.006%)
0.5 -> 0.55 : 0 (0.000%)
0.45 -> 0.5 : 18 (0.009%)
0.4 -> 0.45 : 15 (0.008%)
0.35 -> 0.4 : 0 (0.000%)
0.3 -> 0.35 : 4 (0.002%)
0.25 -> 0.3 : 4 (0.002%)
0.2 -> 0.25 : 0 (0.000%)
0.15 -> 0.2 : 0 (0.000%)
0.1 -> 0.15 : 0 (0.000%)
0.05 -> 0.1 : 0 (0.000%)
0.0 -> 0.05 : 8 (0.004%)
and for Max. Angle:

Code:
Min = 90, max = 179.999, mean = 97.9321276749
194306 elements with the "Max angle" diagnostic
Histogram of Max angle values
171.0 -> 180.0 : 8 (0.004%)
162.0 -> 171.0 : 0 (0.000%)
153.0 -> 162.0 : 0 (0.000%)
144.0 -> 153.0 : 0 (0.000%)
135.0 -> 144.0 : 0 (0.000%)
126.0 -> 135.0 : 5406 (2.782%)
117.0 -> 126.0 : 9352 (4.813%)
108.0 -> 117.0 : 12414 (6.389%)
99.0 -> 108.0 : 19838 (10.210%)
90.0 -> 99.0 : 147284 (75.800%)
81.0 -> 90.0 : 4 (0.002%)
72.0 -> 81.0 : 0 (0.000%)
63.0 -> 72.0 : 0 (0.000%)
54.0 -> 63.0 : 0 (0.000%)
45.0 -> 54.0 : 0 (0.000%)
36.0 -> 45.0 : 0 (0.000%)
27.0 -> 36.0 : 0 (0.000%)
18.0 -> 27.0 : 0 (0.000%)
9.0 -> 18.0 : 0 (0.000%)
0.0 -> 9.0 : 0 (0.000%)
I tried to run the solver in double precission, but the error still occurcs.
__________________
grid generation: ICEM CFD 13.0
solver: CFX 13.0
Julian K. is offline   Reply With Quote

Old   November 17, 2011, 08:43
Default
  #15
Senior Member
 
Julio Mendez
Join Date: Apr 2009
Location: Greensboro, U.S.A
Posts: 106
Rep Power: 8
juliom is on a distinguished road
Send a message via Skype™ to juliom
Dear friend,
The mesh is not the problem, I read your mesh file and it looks very well.
I think you have to make your simulation smoother, I mean start using a first order for momentun and the other variables. Then start making your simulation more real, changing to second order or more.. BUT first of all check your boundaries conditions...
juliom is offline   Reply With Quote

Old   November 17, 2011, 10:24
Default
  #16
Member
 
Julian Krick
Join Date: May 2009
Location: Guelph
Posts: 88
Rep Power: 8
Julian K. is on a distinguished road
Quote:
I think you have to make your simulation smoother, I mean start using a first order for momentun and the other variables. Then start making your simulation more real, changing to second order or more.. BUT first of all check your boundaries conditions...
Thanks Juliom for your help!

My boundary conditions should be okay. My simulation has been running for more than 700 time steps before this error occured and the residuals slowly decrease. From this, I assume that I don't have a convergence problem.

The error occurs, when the solver tries to write the backup-file. From time step 0 to 700 the simulation ran in double precision mode. From time step 701 to 735 (when the error occured and the solver wrote the backup file), the simulation ran in single precision mode. Unfortunately, I am not able to run the solver in double precision mode when I use the switch argument -continue-from-file (there is some problem with my system).

Thus, I assume, that the error is caused by the single precision mode. I will try to run it in double precision and post the results here.
__________________
grid generation: ICEM CFD 13.0
solver: CFX 13.0
Julian K. is offline   Reply With Quote

Old   November 17, 2011, 17:03
Default
  #17
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,937
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Sounds like a numerical divergence caused by the extra numerical round-off errors with single precision.
Julian K. likes this.
ghorrocks is online now   Reply With Quote

Old   November 18, 2011, 10:18
Default
  #18
Member
 
Julian Krick
Join Date: May 2009
Location: Guelph
Posts: 88
Rep Power: 8
Julian K. is on a distinguished road
I managed to solve the problem. I am now running CFX in double precission mode and the solver has no problem when writing the backup file.
__________________
grid generation: ICEM CFD 13.0
solver: CFX 13.0
Julian K. 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



All times are GMT -4. The time now is 07:04.