Hi all,

I'm currently modeling 3d supersonic, compressible, inviscid external flow. The grid is quad. BCs: pressure far field and a simmetry plane. By now I was able to model successfully subsonic and nearly-sonic flows by means of coupled explicit solver. I tried even with the implicit but Fluent just hanged, probably due to the fact that my mesh is of millions of cells.

Now I want to increase the Mach number of the flow to 3 (fully supersonic), but the solver diverges. I played around with parameters following suggestions from tutorials or UGM documents without success. I even switched to segregated but with my great surprise the solver hangs just like in the coupled imp case...it does not even complete the first iteration.

Any hint?

Thank you in avdvance

Edi.

Coupled solver is better for supersonic flow than the segregated solver. You'll get better refinement of the shock, and it is more stable.

For supersonic flow (it was a 'wedge' or something like that, right?) you should use the Coupled solver, with some mesh refinement for the mach cone. Solve it using the first-order solver, then after you've reached a reasonable level of convergence (doesn't have to be fully converged... maybe 100 or 200 iterations) you can switch to the second order solver. Lowering the Courant number (also called CFL number in the tutorials and this forum) will make the model more stable, but will increase the number of iterations needed to converge. Your biggest concern should be in your mesh though. Make sure you have some refinement for the mach cone, as well as wherever you would get an expansion fan. You can use the grid adaption tool, but only to a certain extent. If you adapt the cells too much, then you'll have problems with convergence because you'll have large cells right next to extremely small cells.

Coupled solver will use about twice the memory as segregated solver. If you're running on a single processor (assuming it's a 32bit process, you're limited to 2Gb of RAM per process no matter how much is in your computer) then you're limited to about 800,000 to 1million elements with the coupled solver while with the segregated you can probably run about 1.6million. If you try to run a larger mesh then you'll go to 'swap space' which is your hard drive, and it will seem like your process is hung up but it really is running... just EXTREMELY slow. If your mesh is over 800,000 then you should probably switch to segregated solver. If this is the case, let me know and I'll give you recommendations for solver settings and such. If you're running in parallel, then you should limit yourself to about 800,000 / processor with the coupled solver and 1.6million with the segregated.

Hope this helps, and good luck, Jason

You're absolutely right when you say that the coupled solver is better than the segregated solver when dealing with high-velocity compressible flows, I just tried to have an initial guess with the segregated to switch to coupled afterwards and I was really surprised to see that the solver hung up (or it was extremely slow): doesn't the segregated solver require less memory than the coupled one??? In the end, playing with the courant number, setting reasonable limits and using a previous subsonic solution as an initial guess I was able to find a "solution" using a coupled explicit scheme for the supersonic case, but my mesh definitely needs a refinement...

Thanks again

Edi.