Hello,

I have been working with ansys cfx awhile now, and I still have no idea It is very frustrating. I am running a series of multiphase isothermal transient problems. Typically I have air as my continuous phase with solid dispersed particles as my second phase. I use the kinetic theory, which I understand is very unstable in the solver. Depending on my geometry, sometimes I obtain a solution and sometimes the solver crashes. When it does crash, I get the same error EVERY time;

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

When I track back through the solver out file, there doesn't seem to be any reason why it crashes. The u,v,w velocities for both phases display OK although sometimes P-vol only has ok. I have had some success with decreasing the timestep, but it is just trial and error. I don't understand why I am picking which value. This method is also time consuming as I decrease timestep, let simulation run until it crashes, decrease timestep again, etc etc.

Also, when I open the last outputted transient results for a crashed simulation, I don't really know what to look for. The velocity and pressure distributions seem ok.

Does anyone have any general advice?

Thanks, Tim.

Depending on the models you use, the behavior can be very unstable. One of the current simulations I'm running has taken several attempts to get it working. Best advice I have:

- Use a high quality, reasonably fine hexahedral mesh. - Be sure y+ is good enough to adequately resolve boundary flow - Start from a very well-converged initial state, if applicable. I use RMS 1E-5 as my convergence criteria. - At the beginning of the transient, use very small time steps with very tight convergence criteria. I use RMS Courant number < 0.5 with 1E-7 convergence criteria, max 10 coefficient loops - Increase time step manually and loosen convergence criteria a little after 20 or so time steps. - Make sure your Courant numbers aren't too high. Large time step size can lead to unstable behavior. - Select the option in Pre to output residuals. Regions with high residuals can indicate mesh quality problems.

First steady,then transient,i think.

Hi Andrew,

Thanks for your response, you have some good points in there I have taken on board. A method I have trialled today is that I have solved the problem using the upwind scheme (1st order) and then I have used the solution for this as initial conditions for solving the high resolution scheme. This has worked today for a couple of problems where trying to solve the problem using the high resolution scheme straight away (with zero velocities in domain for initialisation) has not worked. I guess this leads to the conclusion that initial guesses are very important.

Tim.