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

Error #001100279 (floating point overflow)

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 5, 2009, 20:04
Default Error #001100279 (floating point overflow)
  #1
Reza
Guest
 
Posts: n/a
Hi all,

I think this error has been reported many times, but as far as I have ssen in the previous topics, they get the error during the solution or even before that. My problem is a bit wierd, solver finishes the solution, the residuals are at very good levels: (from the *.out file)

CFD Solver finished: Wed Mar 4 00:23:43 2009

CFD Solver wall clock seconds: 1.0533E+04

Execution terminating: all residual are below their target criteria.

and solver starts to give some statistics on all equations, forces, maximum residuals and their locations, and CPU requirements, and then,

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

I'm using the 2 equation transitional SST model, and I use the fully turbulent SST as the initial guess. at the end, my momentum, and mass conservation residuals are under 1e-7 and my turbulent residuals are under 1e-6, the intermitency residual is about 2e-4, and the turbulent onset Reynolds number equation residual is about 1e-5.

The solution ends because I couldn't find how to set the criteria for intermittency and Retheta equations, so as soon as the others go below their criterias solver ends the solution, and I usually check the solution and let it go untill those residuals get small enough. But with this new grid I get this error.

Solver is able to write a res file, but it doesn't have all the variables (it misses variables like y+, wall shear, ...) and the most important thing for my study is wall shear *_*

y+ values of the fully turbulent solution are below 0.7, and the expansion factor near the wall is 1.05. I will gladly provide more information if needed.

Thank you for your time, and I really appreciate if someone can help me out of this problem.

Thanks, Reza.
  Reply With Quote

Old   September 23, 2009, 12:30
Default Error #001100279 (floating point overflow)
  #2
New Member
 
Kambiz
Join Date: Mar 2009
Posts: 5
Rep Power: 8
kamnaz is on a distinguished road
I have the same exact problem. Were you able to find any solutions for this problems or at least the cause of it?

Thanks.
Kam
kamnaz is offline   Reply With Quote

Old   September 23, 2009, 18:55
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,960
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
This error is usually caused by a divide by zero. Normally this happens in the solution but if it is happening for you after the solution is finished and it is cleaning up then you have to do some investigation to find it.

What is the part of the output file it crashes in? My guess is that part (or the part which follows it) is not properly defined and leads to a divide by zero error. Maybe you have some additional variables or CEL causing the problem.
ghorrocks is offline   Reply With Quote

Old   September 24, 2009, 07:13
Default
  #4
Senior Member
 
Join Date: Mar 2009
Location: Europe
Posts: 168
Rep Power: 8
joey2007 is on a distinguished road
Looks like something is going wrong while you are writing the res-file. I had such an issue with CEL expression which fails on boundaries some month ago. The support told me, that the solver tries to write out to the result file as much as possible. If the solver fails while calculating your variable, he skip it and tries the next. This behavior safes the rest of the result.


In your case the solver fails to write turbulent values. So check all setup parts dealing with turbulence. Another check would be what happens when your writing full backups or full transients results?
joey2007 is offline   Reply With Quote

Old   September 24, 2009, 15:15
Default Double Precision is the Solution
  #5
New Member
 
Kambiz
Join Date: Mar 2009
Posts: 5
Rep Power: 8
kamnaz is on a distinguished road
Thanks for the notes. I have two gap regions in my model of 1 micron clearance (jets) while the characteristic length of the model is 10cm or so. The single precision solver failed to address this but switching to the double precision solver took care of my problem.

Thanks again,
-Kam
kamnaz 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


Similar Threads
Thread Thread Starter Forum Replies Last Post
ERROR: Floating point exception: Overflow Elisabetta CFX 19 March 30, 2015 06:34
Error:: Floating point overflow arunraj CFX 7 February 8, 2012 05:58
block-structured mesh for t-junction Robert@cfd ANSYS Meshing & Geometry 20 November 11, 2011 05:59
Floating point exception: Overflow? mike CFX 4 December 15, 2009 18:30
Gmsh and samplesurface touf Open Source Meshers: Gmsh, Netgen, CGNS, ... 2 December 10, 2007 03:27


All times are GMT -4. The time now is 11:29.