Hi,Every one,

I need to simulate the usteady flowfield of 3 blade rows with the blade rotating speed equal to 0.0, -8000, +8000. Is Fine/Turb6.1 suitable for fulfilling the work? In fact, I have simulated the unsteady flow field by using this software, but I could not be convinced with the results. The time averaged efficiency of unsteady simulation is lower than that with steady simulation by 2-4 percent. This is some what inconceivable because the steady method often gives additional numerical loss at mixing plane. Though my researches show that the flow undteadiness always bring out loss, I still can not believe that there is so much difference in efficiency between steady and unsteady results.

BTW, the out flow velocity of the second blade row is very high, namely about 1.5 Mach.

Thanks in Advance for any replys.

Ji

Dear Ji,

This case seems to be very interesting, including counter-rotating components.

Results obtained with the steady and unsteady versions of the solver should be very consistent, as they are based on exactly the same solver. The only difference lies in the rotor/stator boundary condition treatment.

You are right when mentioning that steady state mixing plane interactions may introduce some losses. The Numeca solver ensures strict conservation of mass flow, momentum and energy. But conservation of entropy cannot be strictly ensured and depending on the configuration the mixing induces some losses.

The unsteady rotor/stator boundary condition becomes a single connecting boundary condition, based on interpolation procedures. Apart from interpolation errors there is no loss introduced. Numeca recently published unsteady results obtained by Snecma on the turbopump of the Ariane 5 engine, showing very close correspondence between calculated and measured time dependent pressure profiles (Proceedings of the IAHR conference, Lausanne, Sept. 2002).

By the way did you verify the following features ?

- Is the periodicity of the mesh strictly identical on both sides of the interface ? - Is the number of time steps sufficient ? (the parameter NOFROT should be set to at least 12) - Did you ensure convergence of the calculation at every time step (Number of inner iterations should be sufficient, 20 to 100) - Is domain scaling activated (IDOMSC=1) ?

- Did you test the influence of the turbulence model ? Our recent experience shows that at transonic flow conditions Spalart/Almaras better predicts shock/boundary layer interaction.

Do not hesitate to re-contact us for more questions.

Alain Demeulenaere

Numeca International

FINE/Turbo Product Manager

Dear Alain Demeulenaere

All the features you mentioned are correct in my calculations. Moreover, I think turbulence model could not introduce so much difference, e.g. between the time average flow masses at inlet and at outlet. also I am not able to analyze that the efficiency is lower than that obtained with mixing plane method for about 2-3percent.

ji

Hi Ji, Except for the tubulence model, as Alian suggeted, I would like to know the efficience difference is at one working point or in the whole performance line? If is at one point, I would suggest you to run few more points and compare the performance line, instead of only one points, as the working points compuated with steady and unsteady may be different. best,