Vladimir, There are some points that you can check to obtain better results:

- Check in solver control if you are using the high resolution advection scheme and turbulence numerics.

- Use more numbers of iterations. Set the maximum 1000 (ou higher), instead the 100 you are using. Probably, just 100 is not enough. In many case, the residual declines afer a rise.

- Use small number for the residual targed (1e-5, for example)

- Use conservation target of 0.01. This will ensure a domain mass imbalance less than 1%.

- Check the appropriate turbulence model for your case.

- Check the mesh. Refine the elements close to the walls.

1. Use more numbers of iterations.

2. Use small number for the residual targed

3. Use conservation target of 0.01. This will ensure a domain mass imbalance less than 1%.

4. Check the appropriate turbulence model for your case.

The first and foremost important thing is to improve convergence : in particular the density residual is directly related to an error in mass conservation and therefore the difference in mass flow rate.

Improving the accuracy of the scheme is not going to help you: also the low precision scheme should conserve mass. Therefore, I would advise you to converge fully with the low acuracy scheme and then switch to higher accuracy.

But the most important thing is to check what could hinder your convergence. Possible reasons are

- an intrinsically unsteady flow, often due to large separations. In this case, you will never converge a steady computation and you have to switch to unsteady computations

- a badly conditioned mesh : your solver should give you measures of the quality of the mesh. If it is bad, try to improve the mesh first.!

Willian Andreão , Dušan Regodić , thanks for the advices ,but unfortunately they didn't help.I always use conservation target of 1%.I increased the maximum number of iterations and established RMS 1E-5. Howewer, even after 100 iterations residuals continued to increase , untill Solver Manager completed work with error:

OUTER LOOP ITERATION = 175 CPU SECONDS = 1.426E+04

----------------------------------------------------------------------

| Equation | Rate | RMS Res | Max Res | Linear Solution |

+----------------------+------+---------+---------+------------------+

+--------------------------------------------------------------------+

| ERROR #001100279 has occurred in subroutine ErrAction. |

| Message: |

| Floating point exception: Overflow |

| |

| |

| |

| |

| |

+--------------------------------------------------------------------+

+--------------------------------------------------------------------+

| ERROR #001100279 has occurred in subroutine ErrAction. |

| Message: |

| Stopped in routine FPX: C_FPX_HANDLER |

| |

| |

| |

| |

| |

+--------------------------------------------------------------------+

+--------------------------------------------------------------------+

| An error has occurred in cfx5solve: |

| |

| The ANSYS CFX solver exited with return code 1. No results file |

| has been created. |

+--------------------------------------------------------------------+

Vladimir Dorofeev, try to refine your mesh. Check if the outlet boundary condition is set correctly. Which turbulence model are you using?

Another option is simulate using transient condition.

Floating point overflow indicates that a variable of a cell approaches infinity. Look at the last step available and find the cell and variable causing the problem. This will point to the root cause of the numerical instability and also potential problems with mesh quality.

The turbulence model used should be appropriate for the problem

The mesh must be very refine (smooth) in this zone (turbulent zone)

employ a high numbers of iterations, and gives the software enough time to reach the solution for converge

I would make more cells on sharp edges where turbulence starts and in turbulent areas to see how results change and to eliminate this cell size factor as contributor

Willian Andreão , Koen Hillewaert , Dušan Regodić , Sven Rechenberger , Abbas J Jubear , Radoslaw Koneczny thanks you very much for the advices.

I think i guessed what is happened here.I noticed,that when calculating half closed valve, there are places where the working fluid reach's supersonic speed (fig.1). When calculating fully open valve the fluid has subsonic speed.

I thint think that is logical, because total presure and temperature are constant at the inlet.

To check this out i made the calculations for the cases beetween fully open valve and half closed valve. Turns out that i found adequate solutions only if fluid has subsonic speed.

And now i got another question : from course of fluid dynamic, i know that waves of impulses in the subsonic fluid and in the supersonic fluid has different distributed. For subsonic fluids this is explained using so-called "suntop" system of equations,for supersubsonic fluids this is explained using so-called "hyperbolic" system of equations.

I think that when Ansys CFX solver calculating cases with supersonic speed he uses "suntop" system of equations and because he can not found adequate solution.

Please can you tell me how to set "hyperbolic" system of equations in Ansys CFX ?

Thank you all for the advices. I've finally found the cause of my problem. In the first calculations half closed valve, i set up the following boundary conditions: at the inlet - total pressure and total temperature, at the outlet - mass flow rate.

Numerical value of mass flow rate i get from my assumpitions. But it turns out that my assessment of mass flow rate was wrong. 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.

This problem i solve by this way: the moment when the residuals start increase i stopped the calculations. After that i modify boundary conditions at the outlet : i set up the value of static pressure instead the value of mass flow rate. The numerical value of static pressure i get from first iterations. After that i continued the calculations . In this case, all residuals start decreasing, Ansys CFX corrected mass flow rate at the outlet and finally i get adequate solution.