ERROR #001100279 has occurred in subroutine ErrAction. Message: Floating point exception: Overflow

What does it means? Can anyone help me? Thanks a lot.

Well,

This tells you that your solution is diverging and obviously it depends upon your simulation setup, there could be many reason as you have not mentioned what you are doing?

Alice,

This refers to your mesh size as well as simulation time step. Optimize your mesh size and timestep so that your solution don't diverge.

Change the scheme on Solver Tab.

Steady State simulation, the scheme is Upwind. Is a 8 million elements mesh, tetra + prism. PC configuration: Intel Core 2 Quad Q6600 2.4 Ghz 8 GB RAM DDR2 PC800 Kingston

Is the mesh too large? I´m new in CFD Realy thanks for the help guys

try to reduce (element number) a little the mesh or use hexa mesh, if it´s possible! Are you using Linux 64 bits with CFX 64 bits? If not, start using!

I´m using windows xp 64 bits. i´ll try this, thanx for help

This error message can occur for many reasons! We don't have much information to go on, soI would guess that either there is a problem with the model (bad combination of boundary conditions, etc), the mesh (have you checked the mesh quality?), or the initial conditions. That covers everything and anything!!! ;-)

1) When did this error occur? If it happened on iteration 10, then re-run the simulation for just 8 or 9 iterations and look at the results. The results just before the crash might show where things are going wrong.

2) Try and start from a coarser mesh. An 8 million cell tet mesh is quite large. It is normally much better to perform a simulation on a coarser mesh with fewer cells, then use the coarse results as an initial guess for the fine mesh. Have you done this?

3) If necessary, use a simple turbulence model initially to get some results, then use these results to start a new simulation with the correct turbulence model.

4) Read the CFX Help documentation - it contains lots of tips about dealing with convergence problems.

5) Simplify the model in as many ways as you can, until it starts working, then gradually add all the details back in, carefully....

6) What timescale is CFX using for your model? Use a small timescale for the first few iterations.

7) Give us more information if you want further help! (If you have a CFX support contract, contact them - you will get a faster response!)

Good luck, Andy

Now i know what is the problem. i was using too small height of prism, and the transition between the prism layer and tetra elements wasn´t good. Now i have another problem: how can i get a good value of y plus with a not too large mesh (i gave up the 8 million mesh!) I´m working with a simulation of tubular reactor, i was using prism height 0.1% of diameter, 10 layer, but it doesn´t work. I´ll keep trying Thanx a lot!