Floating point error?????
 

When I try to run the simulation on a 2-D rocket nozzle, Fluent says "floating point exception (imprecise)".Does anybody know what that means? thanks in advance, -kiran

Re: Floating point error?????
 

it means we shall wish you best of luck. god knows the behaviour of fluent ..if u take this case to other machine this error might even go for the same case.

Re: Floating point error?????
 

hi, you check meshing and bcs is not accurate nabeel

Re: Floating point error?????
 

Hi,

wrong boundary condition definition might cause the floating point error. For example setting an internal boundary as interior.

Another reason could be a to high courant number - that means, that the steps between two iterations are too large and the change in the results is too large as well (high residuals).

Once I had the problem, simulating a 2D chamber with a symmetry BC. I set the symmetry somewhere as "axe symmetric" and the floating point error occur.

Ralf

Re: Floating point error?????
 

Hi, its me again!

The floating point error has been reported many times and discussed a lot. Here are some of the answers I found in the fluent Forum:

SOLVER AND ITERATION -----"I think if you set shorter time step, it may be good. Or changing little Under-Relaxiation-Factors, it may be good. In my experience, I set 1/3 Under-Relaxiation-Factors as default." -----"also lower the values of under relaxation factor and use the coupled implicit solver" -----"Try to change under-relaxation factors and if it is unsteady problem maybe time step is to large." -----"you can improve the ratio in the solve--control--limits, maybe that can help." -----"you will need to decrease the Courant number" -----"If you still get the error, initialize the domain with nothing to 'Compute from...' Then click 'init'. Again select the surface from which you want to compute the initial values & iterate. This should work." -----"Another reason could be a to high courant number - that means, that the steps between two iterations are too large and the change in the results is too large as well (high residuals)"

GRID PROBLEMS -----"this error comes when I start scaling grid. in gambit, all my dimension is in mm, when in fluent i convert it in meter using buttone SCALE. after it, when i iterate, about hundred iteration, this error appeared. but when i not scale my drawing to m...and let it be as in gambit..then the iteration is success. -----"hi I think you should check your mesh grid mesh is very high. your problem solve by selection a low mesh." -----"Your mesh is so heavy that your computers resources are not enough. try to use coarser mesh."

BOUNDARY CONDITIONS -----"In my case I had set a wall boundary condition instead of an axis boundary condition and then FLuent refuses to calculate telling me 'floating point error'." -----"Your Boudary Conditions do not represent real physis." -----"wrong boundary condition definition might cause the floating point error. For example setting an internal boundary as interior" -----"Once I had the problem, simulating a 2D chamber with a symmetry BC. I set the symmetry somewhere as "axe symmetric" and the floating point error occur" -----"check the turbulence parameter you set. reduce the turbulence intensity to less that one for first, say 50 iterations.

USING A UDF -----"What I mean is really often when people creates UDF they generally forget that for the first iteration some variable can be zero. Therefore if you are divided a number by zero your solver will blow up telling you 'non floating error'. 'non' means 'not a number'. Depending on your UDF this kind of error does not effectively happens at the first iteration. An example, if you are simulated a domain with a stagnant water as initial condition and you are calculated for the first iteration something like 1/Re therefore lets call it BOOM !!! because Re=0 . To find this kind of think there a simple way : reread your UDF."

MULTI PROCESSOR ISSUES -----"I've had similar problems recently with floating point errors on a multi processor simulation. The solution for my problem seems to be to run on a single processor, where it runs fine....?"

-

Re: Floating point error?????
 

about multiprocessor issue: i wi sh to say something here .. i also noticed that error on my two processor machien if i read the case in parallel fluent, while reading the mesh file ..but the same file is easily read by single processor fluent (or non parallel fluent) ...anyway i had to mesh that case 4-5 times and i kept on trying to import the mesh ..finally i was able to read it with same tricks (i have forgotten them) ... but it seems the problem was coming due to defination of a fluid zone (i mean i named one fluid zone ..so that i can use it with slidign mesh) .... in all double processor fluent has a problem ..