I haved the same problem when i calculating valves for steam turbine in Ansys CFX.

I used boundary conditions: Total Pressure and Total Temparature at the inlet and Mass Flow Rate at the outlet. Working fluid is Water Ideal Gas. In this case i got solutions when i have subsonic speeds of the flow (Mach number less 1).

But i can not got solution when i have supersonic speed of the flow (mach number more than 1). As and you i have error Floating point exception: Overflow .

The problem was very simple: numerical value of mass flow rate i get from my assessment. But it turns out that my assessment of mass flow rate was wrong. Real critical mass flow rate was smaller than the mass flow rate ,which i set up at the outlet boundary conditions. In the first iterations, residuals decrease untill the mass flow rate at the inlet equal to the critical mass flow rate. After that, residuals start increase, because the mass flow rate at the outlet is boundary conditions (more than critical mass flow rate) and Ansys CFX can not modify it.On the other hand, the mass flow at the inlet has already achieved the critical value and because Ansys CFX can not increase it.That was the reason of my problems.

to check it i advise you use User Monitors for Mass Flow Rate at the Inlet. If i am right when you will be calculating you will see that value of Mass Flow rate at the Inlet stabilize at the value which will be less that value of boundary conditions Mass Flow Rate at the Outlet. That will be mean that you try blew through your turbine Mass Flow Rate which more that critical Mass Flow Rate.

So I think that the your turbine can not miss enought mass flow rate to achieved 100 KW.

I think first of all you need determini maximum mass flow rate for your turbine. Try use User Monitor Point for Mass Flow at the Inlet. When you will see that Mass Flow rate stabilize at the value that less your boundary conditions at the outlet stop the calculation. Start another calculations but at the outlet define Mass Flow rate with value equal Mass Flow Rate at the Inlet from first calculation. Do it untill you get solution.

After that you will see how much mass flow rate additionally need pass through your turbine to achieved 100 KW.Based on this data you have to change angles blades of turbine to do that your turbine will can pass enought mass flow rate.

But i am getting the same error when i tried to run the simulation on 50 Kw turbine also with inlet boundary condition as pressure and outlet as mass flow rate.

Dinesh Kumar , it means that you defined too much mass flow rate at the outlet.

You can check it. You have to look how much mass flow rate pass through outlet in the successful calculation with static pressure boundary condition at the outlet. If i am right you will see that value of this mass flow rate less than value of the mass flow rate when you calculate with mass flow rate boundary condition at the outlet.

Vladimir Dorofeev Thank you so much for your answer.

I have another query that during the meshing i am getting an error in mesh statistics regarding Maximum Edge Length Ratio. 2400 approx with 0.25 bad %.

and as i increase the mesh factor numbers of nodes reaches 4 million and Maximum Edge length ratio reaches. 1400,

now my query is does this Maximum Edge Length Ratio produce some effect on the convergence or Efficiency.

Dinesh Kumar Of course,mesh quality is important ,but first you have to define physically correct boundary conditions.

For turbomachinery, they usually use special programs to create quality mesh. In Ansys there is Turbogrid. In this program you can easily create quality mesh for turbomachinery. The most popular method to create mesh for turbomachinery in Turbogrid is Y+ method.