error in fluent
 

hi all,

whats meaning,
divergence detected in AMG solver: w-swirl ,not converging.
Error Object: ()

grid - bc - numerics
 

That means that there is s.th. wrong with your case:
1. A problem with the grid (resolution, too big size ratios, too high skewness..)

2. Boundary conditions are posed in a bad way: e.g. you want to model a water flow but you forgot to change the material, or - happens very often - you forgot to scale the model from mm to m...

3. A problem due to numerics:
a) If you use the segregated solver (pressure based) try to reduce your under relaxation parameters (momentum to 0.3 pressure 0.1 k-eps 0.4; energy 0.95 ..) and observe the residuals; maybe go one step further and try to get a "first" solution with 1st order discretization instead of second/third and then switch to 2nd again.

b) If you use the coupled solver (new terminology: density based): try to lower the CFL number (but I think, AMG corresponds to the pressure based solver only..)

w-swirl..: indicates that you're a running a 2d-job? Then try fisrt to reduce w-swirl if it is imposed to the system by you. Increase it parallel to the converging solution.

grid - bc - numerics
 

Hi volker,
Thankyou for replay

i am simulating Tesla turbine one single blade .
please your mail ID will give,i want send my file,and some clarifications.
Thnakyou

Hi sivirama1,
I regret, but I won't have the time to look closely on your case, since I am completely occupied with my own work. Better is to contact your provider. If you can't then at first try to work through the 3 points I mentioned earlier : 1.grid - 2.boundary conditions - 3.numerics Follow that order!

If you are modelling one blade only, you should have periodic boundary conditions in your model? Are they really periodic? i.e. Did you really choose rotational periodic?? Where did you define the periodicity? Inside fluent or outside in your grid generator? If the latter then try to define them via TUI (Text user interface) /grid/modify-zones/make-periodic (I think in fluent 12 it should be mesh instead of grid; noone except for the Ansys managers knows why they:mad: changed it..)
AND: You must define the correct rotation axis. This is done in the cell-zone bc panel where you also define your motion. I am not sure but it might be necessary too to define that zone as a reference zone under report "reference values". The last is at least necessary to postprocess your results relative to your rotation.

I hope this helps a little bit. Unless answer again or contact your key user or provider.