Hi!

I have a 3D Simulation with an incompressible gas that runs pretty good. The gas velocity is low (about 4 m/s) at a Temp. of 300 K. Now I am turning on the ideal gas law â€" with energy equation â€" and initialize the same simulation again. Following error appears:

"absolute pressure limited to 1.000000e+00 in 467560 cells on zone 2"

and then, when I begin iterating it says something like:

"temperature limited to 1.000000e+00 in 160 cells on zone 2 in domain 1" absolute pressure limited to 1.000000e+00 in 7 cells on zone 2 turbulent viscosity limited to viscosity ratio of 1.000000e+05 in 13 cells"

and after 3 or 4 iterations :

"divergence detected in AMG solver: temperature Primitive Error at Node 0: floating point exception"

And that's it! What is the problem??? The geometry is not so complex. I had almost the same error in a totally different geometry…

How can I avoid this error???????

Any help is highly appreciated

r u not running this with coupled solver ?????

You are right, I was using the segregated solver…

Now I was trying with coupled solver. But implicit as well as explicit are giving similar results… Fluent is not even iterating any more… before the first iteration finished it exits. Even when turning the currant number from 1 to 0.1

How about increasing the limits? Even if these limits are beyond what you expect in your physical domain, just remember this is a numerical simulation and during the convergence process a lot of things take place that might lead to these high pressure or temperature values.

its difficult to say much from this side, but if you can get some solution without turbulence model on. and if you see some convergence then it is clear that making the turbulence model on, is cousing the problem. Since it write the warnign about viscosity ratio . I were you, i could have tried this:

Save the initial guess, from incompressible converged solution, then go to the compressible version, and use very conservative urf for k, e, around 0.5, and 0.2 for viscosity. Then go the control, multigrids, change the cycle type to W for k and e. increase the post interations for fixed cylce for fixed cycle to 3-4, and increase the flex clcyle post interations to 3 from 1.

(if you wish you can change cycle type of pressure to W also from V)

Now we have a very conservative solution approach, (use first order schemes for momentum and k and e in the start of iterations, you can later on switch to second order schemes).

even after that you do not get the convergence, we might have to look into whole case again

Hi!

Thanks a lot for your answers, but it still doesn't work…

I made all the settings you suggested, set the viscous model to laminar, set the limits to there maximum and used seg. as well as coupl expl and impl. solver. Also courrent number is set to 0.1.

But only the segr. solver seems to give one iteration, the others are stopping in the first iteration. Might it be a different kind of problem?? There is no floating point error or something. What happened is that in the first iteration the "connection is refused" to the computer. So could this be the problem???

Ralf

i do not think that u r doing the parallel calculations. Yes if it is still giving this problem then there might be some set up problem, i am not sure what but it definitely means probs other than solver. Because as a solver fluent is very robust, i am not able make it diverge till now on any case properly set up (this means that i have made the case to diverge with same settings on other solvers like starCCM+). it does not soun like solver prob.

If the flow is not compressible, why r u using ideal gas, use incomp.ideal gas either.

This is just the first step... For the simulation of my experiments incompressible gas without temp. changes is enought.

For simulating the real cases, temp. changes and pressure is quite important. So i am stll on it... will report on my progress. Ralf

I got it!!

The problem was either that I separate my geometry in two half (partitioning) or (and that's more likely) that I set the reference pressure to 0…

That works fine for incompressible simulation returning the pressure I need for calculations… But â€" and I admit that was pretty stupid â€" not for compressible of course… Now it seems to work… but Fluent failed to allocate memory… that's another problem…

Thanks so far for your help!

Ralf

Go to solve-> controls -> limits. Change the minimum limits to 1kpa for pressure and 298 (or sth) for temperature and run it for some simulations. Then switch back to the defaults later on. It takes some time to adjust to physical solution.

Hyde

Goof up. I mean run it for some iterations. EOM