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

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.

hi, you check meshing and bcs is not accurate nabeel

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

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....?"

-

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 ..