hello I have to study the flow around an aircraft at different Mach number, I have created the mesh with gridgen but the simulation with fluent diverge for all my cases!! my simulation is a compressible, inviscid, steady calculation, with pressure far field boundary conditions and wall condition for the aircraft. The mesh has 1.5 million cells with a max aspect ratio of 6.3 and a max volume skewness of 0.93. I have checked my parameters, and the simulation converges for a first order calculation but as soon as I try the second order the calculation diverges. I really need these results for my Msc thesis... thanks vincent

What Mach numbers are you running? What solver and solver settings are you running?

If the solution is diverging, then there is typically a region where the flow field is falling apart... look at the diverged solution and find that area (look at Max/Min pressures, temperatures, and Mach numbers). In that region is the mesh refined enough to capture gradients (either due to shocks and/or curvature)? Is it diverging in the same area as the maximum skewed cell?

A typical response is to check your under-relaxation factors. That may keep your model from diverging. Personally, I think it's extremely important to understand where and why you're having a problem before trying that, but more and more people seem to jump to playing around with URFs first.

Hope this helps, and good luck, Jason

thank you for a so quick answer I am using a coupled, implicit 3D solver for Mach number from 0.7 to 1.2 Actually when I look at the part where there is a divergence it seems taht this is always the same place but I have already tried to refine the mesh on that particular place (where there is a strong shock wave) and the result is the same. Furthermore this palce is not the place where there is the maximum skewness About the URFs I do not know how to use it, my divergence seems to be about temperature and pressure. Will it affect the accuracy of my results?

For a coupled solver, the next thing I would try (after finding the problem and refining the mesh, which you've done) is lowering the Courant Number (CFL number). You can find the CFL and the URFs in the Solution Control window (Solve->Controls->Solution). The default is 5, so I would try dropping it to 1, and if that still doesn't work, 0.1. The key is to slowly raise the CFL number again if the model is behaving (i.e. if the residuals are decreasing).

Another thing you can try is setting the solution limits, so that the pressure and temperature are bounded and don't go off to extremes (the default temperature will go all the way to 1K... I seriously doubt you're modeling anything that gets that low). You need to leave some "slop" in the available range, but bounding the problem will sometimes help keep the solution from diverging. In my experience this is hit-or-miss with the coupled solver (but always helps with the segregated solver) so it's worth a try at least.

Hope this helps, and good luck, Jason