[ghorrocks]

OK, so if we suspect the SST model is inadequate then you should move to models like SAS and DES. You don't have to develop these models yourself, they are included in CFX (but they are not available to some entry level ANSYS licenses). If you decide to use these models you don't simply turn the model on and they work - they have implications on meshing, boundary conditions, making the model transient and so on.

[Opaque]

Originally Posted by LiuYD

Thank you for the explanation. I have already tried this in CFX-Pre, and unfortunately, in my case I cannot use "exit corrected mass flow". Because my working fluid is an organic vapor, I handle the fluid properties by importing an RGP table. It seems that once the RGP table is used, the option for “exit corrected mass flow” disappears from the outlet boundary condition.

When I switch the working fluid to the built-in air property in CFX, the “exit corrected mass flow” option becomes available.

So, may I ask if you know any method that would allow me to use "exit corrected mass flow" while still using an RGP table for the fluid properties?

Set it as Air ideal gas, set the Exit Corrected Mass Flow option, reset back to your material, ignore the warning/error, write the definition file and see if it works.

[LiuYD]

Originally Posted by Opaque

Set it as Air ideal gas, set the Exit Corrected Mass Flow option, reset back to your material, ignore the warning/error, write the definition file and see if it works.

hi Opaque
The method you suggested works — the calculation can be performed. Using exit corrected mass flow also shifts the location of the sudden jump, but the discontinuity still exists. I have shown the results in the figure below.

In addition, I used the same mesh and boundary conditions in both CFX and Numeca (another CFD solver commonly used for turbomachinery). The results are shown as well. Based on this comparison, we can basically rule out any design issue with the impeller itself. The appearance of the sudden jump is most likely caused by some unexpected numerical behavior in CFX, which leads to a non-physical solution branch.

[LiuYD]

Originally Posted by ghorrocks

OK, so if we suspect the SST model is inadequate then you should move to models like SAS and DES. You don't have to develop these models yourself, they are included in CFX (but they are not available to some entry level ANSYS licenses). If you decide to use these models you don't simply turn the model on and they work - they have implications on meshing, boundary conditions, making the model transient and so on.

Yes, if we use SAS or DES, we will also need to investigate whether specific software settings might influence the results. Since I have been using the SST model and have already obtained some results, I would prefer to solve the issue within the SST if possible — including enabling the reattachment modification and high-lift modification, which I hope will help. Of course, if these still do not work, I will then consider using more advanced turbulence models.

[ghorrocks]

And just checking - are you completely sure that this simulation is fully converged and the mesh is fine enough? What happens if you use tighter convergence or a finer mesh?

[Opaque]

Originally Posted by LiuYD

hi Opaque
The method you suggested works — the calculation can be performed. Using exit corrected mass flow also shifts the location of the sudden jump, but the discontinuity still exists. I have shown the results in the figure below.

In addition, I used the same mesh and boundary conditions in both CFX and Numeca (another CFD solver commonly used for turbomachinery). The results are shown as well. Based on this comparison, we can basically rule out any design issue with the impeller itself. The appearance of the sudden jump is most likely caused by some unexpected numerical behavior in CFX, which leads to a non-physical solution branch.

Would you mind running the BSL model instead of SST? Have not had a chance to digest your previous convergence plots.