Hi

I am having trouble initiating a free stream axisymmetric jet, when i try to iterate fluent hangs and after some time i get the error message: 'floating point error:invalid number'

Additionally when i perform a grid check it fails and reports a non- positive face area, Does anyone know what this means?

I have a rectangular grid 100*600, with an axis boundary and pressure outlet and velocity inlet attached to the axis. The two remaining boundaries are pressure inlet.

I have made sure to place the boundaries far away from each other and made the grid wider and longer than it needs to be.

Any help would be greatly appreciated

Thanks

You should first check your grid in GAMBIT. You will always getting warning messages when you get negative area cells. When you see these messages, you should be certain that this mesh is not acceptable. I do not know what is exactly wrong with your mesh, as it seems to be a rather simple one. Anyway, re-make the mesh and check its quality.

(along what direction is your axis?)

The failed grid check is probably because some of your mesh is below the x-axis. In an axisymmetric case, Fluent uses the x-axis as the axis of rotation, so your model must lie above the x-axis.

This may fix your problem when you try to iterate, if not you may have to adjust your solver settings.

Solver settings are going to depend somewhat on your flow conditions. For a jet velocity up to about Mach 1.3, I would use the segregated solver (if you are doing a supersonic jet and need well defined shocks, then use the coupled solver. The segregated solver tends to dissipate shocks, depending on your grid refinement in the area of the shock, but it's still pretty accurate up to about Mach 1.3-1.5). Use the default discretization scheme at first and change your Pressure URF to 0.5 and your Momentum URF to 0.4. Turn off the turbulence equation (the URF, Discretization, and Equations are all available under solve->controls->solution). Also, it's very important that you set your limits (solve->controls->limits) relatively tight when using the segregated solver. Typically I use Pstatic ± (2 or 3)*Dynamic Pressure as my range for absolute pressure. I also calculate what the Total temperature should be, and I use Tstatic ± 10*(Ttotal-Tstatic) as my temperature range. You will have to adjust your ranges according to your problem, but you should have some rough analytical predictions of what your pressure and temperature range should be, and you can base your limits as being a bit wider than your predicted values. Typically you can usually have loser limits on the temperature range if you're holding the pressure range pretty tight.

After about 100-200 iterations turn the turbulence equation back on and let the model run to convergence (or close to it). Then switch to second order or higher discretization schemes.

The solver settings I've given work pretty well for me for a wide variety of problems. They are not guarunteed to work for your problem, but at least it's a starting point.

I hope this helps, and good luck, Jason

Thanks for your responses guys, the jet is now running. It was quite elmentary in the end and you were both in the right area with regards to the orientation of the axis. I previously had my jet and axis boundary positioned away from the x axis, and as you say Jason, Fluent simulates axisymmetry about the x axis, so that was the cause of the problem.

Thanks again guys