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

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.

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

reply
 

please check your model and mesh carefully!!!

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?

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

reply
 

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 ?

I presume what flyingd meant by 'to check the mesh quality', is to use ICEM to check the mesh.

Could you clarify it flyingd.

reply
 

Yes ,using icme check your mesh quality. If it is not well.
The soft does't calculate.

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.

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)

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

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.

Hi!

I get the same error, when the solver tries to write the backup file:
ICEM output for mesh quality is:
and for Max. Angle:

I tried to run the solver in double precission, but the error still occurcs.

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...

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.

Sounds like a numerical divergence caused by the extra numerical round-off errors with single precision.

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. :)