Turbomachinery Mass imbalance
 

Dear All,

I am doing a simulation of a Axial Turbine stage in CFX Turbomachinery. Turbine stage have 15 stationary blades and 23 rotational blades. My geometry and mesh is 1 stationary blade and 2 rotational blades. Inlet and outlet BC's are Mass Flow at Inlet and Static Pressure at Outlet. Mesh is about 8mln elements. I am performing 200iterations while the residuals stabilizing after about 130 iterations.

After performing a lot of simulations with small rotational blade geometry modifications I found out that ~1.7% of mass was removed from inlet and ~3.5% mass was added at GGI interface. Mass flow is in kg/s.


Example:
MassFlow at S1Inlet = 0.023844
MassFlow at S1toR1 = -0.0238434
MassFlow at R1toS1 = 0.0322807
MassFlow at R1Outlet = -0.0322806


Then to calculate mass flow at interface through entire machine:
S1toR1: -0.0238434 * 15 = -0.357651

R1toS1: 0.0322807 * 23 / 2 = 0.37122805


Mass flow at inlet should be 0.3619



Mass flow at inlet is:
0.023844 * 15 = 0.35766


Imbalance at Inlet:
0.3619 - 0.35766 = 0.00424
0.00424/0.3619*100% = 1.1716% of mass loss at S1 Inlet



Imbalance at GGI interface:
0.37122805 - 0.357651 = 0.01357705
0.01357705/0.37122805*100% = 3.657% of mass was added.


Could You, please explain why the mass flow through inlet is not what I set and why the mass is added on GGI interface?
How could I possibly prevent it?


Best regards,
Oskar

It sounds like your simulation is not converged. In an unconverged simulation the results can show anything.

Your comment ".... the residuals stabilizing after about 130 iterations" suggests this FAQ describes what you need to consider: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

Dear Glenn,


Thank You for Your reply.
I checked maximum Mass residuals by volume rendering and by point for both domains and I think they are pretty good. Please, see the attachments.
I think it is not related to residuals because mass is well preserved within domain. Changes are present at inlet and GGI interface.



Best regards,
Oskar

I think you have confused residuals with mass imbalance.

The mass imbalance is reported in the output file separately from residuals in the flow summary.

You could probably post those here.

Thank You for Your reply.


In fact those numbers are pretty high. Is refining interfaces a solution?

If the concern is a mass imbalance, could you please post the flow summary for P-Mass in S1, and R1? The summary for R1 is missing.

Equation imbalances have nothing to do with mesh refinement. If the solution is converged, the imbalances must be satisfied. The solution may not be accurate because of a coarse grid; however, the imbalance must still be correct.

Thank Your for Your reply.
I think P-Mass for S1 and for R1 is in my previous post. Am I wrong? Are You talking about something different?

Please, forgive me if I misunderstand something.




Best regards,
Oskar

My apologies.. I missed among all the others.

Two things come to mind:
1 - The solution is far from converged
2 - What pitch ratio are you running? The fact that there is such a change when crossing the rotor-stator interface is a sign of pitch change, and the mass flow must be scaled to match the full wheel conservation. Do I make sense

Mass flow at inlet = Mass Flow interface side inlet = Mass Flow interface side outlet = Mass Flow at outlet

Now divide by the number of passages in a given row, and multiply by the number of passage in the model. You should get your scaling factor.

I think this is a solution.
First improvement was to set inlet mass flow 'for component' not 'for entire machine'. Inlet mass flow became good after this. The issue with mass imbalance in between domains is most likely due to automatic pitch ratio and specific connection between stator and rotor domains. See attachment.



I think setting the right pitch ratio between domains will resolve the issue.



Thank You very much.

Your model seems to have a problem on the hub to shroud space.

I can see the pitch ratio scaling from periodic to periodic, but the lip/overlap at the bottom is a wall; therefore, the mass flow either do not fit, or you will get an artificial acceleration due to the area change.

Say you scale the model to full wheel, the cross-sectional area at the interface must be identical, correct? or your machine has a step/lip/contraction when at the crossing?

Thank You for Your reply.


Yes, in fact there is a step change in between rotor and stator domains. I think I need to set Pitch Ratio:

CFX Modelling Guide: "This option enables you to specify the pitch angle on side 1 and side 2 of the domain interface.You can use this option when the precise pitch angle is needed or when the area ratio of the two sides is not equal to the pitch ratio. In most cases, the automatic option is sufficient for determining the pitch ratio."


I need at least 2 days for simulation. I need time to check how those changes influences the final solution. Moreover I need to understand where and why my solution is far from convergence.

I commented on that in post #2. See FAQ: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

Thank You! That was what I meant by saying that I need to figure out how to improve convergence.