[cvh]

Hello all;

I am trying to implement particle breakup due to impingement on walls. I have been trying to use the pt_breakup_wall example user routine that is provided in the examples of user fortran in CFX installation directory. But with particle breakup, the Newton solver seems to fail while calculating total pressure. The continuous phase is modeled using the built-in Peng-Robinson equation of state.

I have tried increasing the number of iterations in the Newton Solver, as well as decreasing the under-relaxation factors, without any success.

I have also tried running the case on a finer grid with smaller time-steps. Also, the simulation runs fine when the breakup factor is kept at 1.

Has anyone encountered this type of problem before? If so, I'd appreciate any tips/suggestions.

Thanks!
cvh

[ghorrocks]

Is the failure due to the particle break up model or the EOS? When you run it with ideal gas as an EOS does it work?

[cvh]

I tried the same case with ideal gas EOS and it seems to work without any issues. So my guess is that it has to do something with the EOS...

For real gases, the properties are calculated by inverting the (h,s) table, so I have tried increasing the number of points in the table. But that hasn'w worked either! I have also tried supplying the initial conditions from the results for the ideal gas case..

[ghorrocks]

If you model the flow with the Peng-Robinson EOS but no particle breakup does it work?

Assuming the problem is the EOS - then you are going to have to use the normal general tricks to improve numerical stability. That means:
* Double precision numerics
* Improve mesh quality
* Improve mesh quality (I repeated this one because it is the most important )
* Smaller time step
* Better initial condition

[cvh]

Thanks for the suggestions Glenn. Peng-Robinson EOS without particle breakup works on my current mesh, and I am already using double precision. I know that CFX calculates real gas properties from the (h,s) table. Also, this error message appears only while writing the backup/results file, and not after every iteration.

Anyways, I'll keep on experimenting with mesh quality and see if that makes any difference.

[ghorrocks]

If the error occurs during writing the results file then there is probably a specific variable in the results file which is causing the problem. If you change to "Selected Variables" and only include the variables you need to use in post-processing you just might side-step the problem.

[cvh]

I increased the coefficients of restitution and now the simulation seems to be working. I think the solver was running into problems while solving for particles near the wall boundaries. Thanks for the help!