Error #001100279 (floating point overflow)
 

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.

Error #001100279 (floating point overflow)
 

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

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.

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?

Double Precision is the Solution
 

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