[LiuYD]

Hi everyone,

I’m running steady-state RANS simulations of a centrifugal compressor in ANSYS CFX. Most operating points converge normally, but near one particular mass-flow value the solution shows a sudden and unrealistic jump.

At around 6.9 kg/s, the results behave abnormally:

The separated vortex structure abruptly disappears.

The flow field changes sharply.

The predicted efficiency suddenly increases.

The behavior is clearly non-physical.

Grid resolution and y⁺ effects are unlikely the cause (already checked). Changing the turbulence model does shift the location of the jump, but the discontinuity still exists at some flow rate.

When I use the solution at 6.7 kg/s as the initial field for 6.95 kg/s, the convergence pattern looks like this:

In the first iterations, residuals drop quickly and key flow variables approach what I would expect physically.

Then, residuals start increasing again.

The solution drifts away from the “expected” branch and finally stabilizes at a lower-efficiency state.

This behavior looks like the solver is transitioning from one solution branch to another, but I’m not sure if it’s a numerical issue or something physical (e.g., loss of stability).

Has anyone encountered similar sudden jumps or branch switching in CFX compressor simulations?
Any suggestions for stabilizing the solution near this mass-flow point or preventing the solver from converging to the non-physical branch would be greatly appreciated.

Thanks!

[ghorrocks]

Are you sure the flow is not choking? That can cause strange behaviour.

CFD results certainly can bifurcate like you suggest. You should be able to use the post processor to see what has changed - the flow has probably separated from a face, or re-attached to another face or some other observable change. Your comment about the turbulence model changing the result at this condition does suggest it is a flow bifurcation.

Also, as your rotor gets further away from the design point you will probably find separations and other undesireable features are dominating. Some turbulence models will not handle grossly separated flows very well, you might need to go to more sophisticated turbulence models for the off design points.

[LiuYD]

Originally Posted by ghorrocks

Are you sure the flow is not choking? That can cause strange behaviour.

CFD results certainly can bifurcate like you suggest. You should be able to use the post processor to see what has changed - the flow has probably separated from a face, or re-attached to another face or some other observable change. Your comment about the turbulence model changing the result at this condition does suggest it is a flow bifurcation.

Also, as your rotor gets further away from the design point you will probably find separations and other undesireable features are dominating. Some turbulence models will not handle grossly separated flows very well, you might need to go to more sophisticated turbulence models for the off design points.

Thanks for your answer!
1.I am certain that there is no surge or choking near the jump point. I have designed several compressors with very similar geometries—for example, sometimes I only change the rotor inlet metal angle by about 1°, and the numerical solution may suddenly show this jump problem. However, in other rotor designs with similar parameters, the performance curves behave normally as expected, and the mass-flow range from 6 kg/s to 8 kg/s shows no issues.

2.In fact, the design point is 7.2 kg/s. Theoretically, as the mass flow decreases, the separation vortex on the suction-side shroud region of the impeller should become more pronounced. But when the sudden jump occurs, I checked the flow fields in CFD-Post before and after the jump. When the mass flow drops below the jump value, the suction-side separation vortex suddenly disappears, which causes the efficiency to increase abruptly. This is very confusing. I am currently using the SST turbulence model.

[LiuYD]

there are some performance curves,one is normal,and the other one have a jump point

[Opaque]

Originally Posted by LiuYD

there are some performance curves,one is normal,and the other one have a jump point

Would you mind posting the convergence plots for the cases on both sides of the jump in efficiency? If you can include all the equations (Cont,Mom,Energy and Turbulence) in a single plot, the better.

[LiuYD]

Originally Posted by Opaque

Would you mind posting the convergence plots for the cases on both sides of the jump in efficiency? If you can include all the equations (Cont,Mom,Energy and Turbulence) in a single plot, the better.

Hello Opaque, thank you very much for your reply! I’m happy to provide these images—hopefully they will help. Let me explain what the figure shows.

In my simulations, I use the average static pressure as the outlet boundary condition. When the outlet static pressure is set to 0.88 MPa, the calculated mass flow rate is 6.587 kg/s. When I change the outlet static pressure to 0.89 MPa, and use the solution at 0.88 MPa as the initial field, the situation shown in the figure occurs. It looks as if the calculation suddenly becomes “idealized”: the residuals drop sharply, the efficiency increases, and the behavior looks very strange. From the flow field, the separation vortex disappears and the flow becomes unrealistically ideal.

[LiuYD]

Originally Posted by LiuYD

Hello Opaque, thank you very much for your reply! I’m happy to provide these images—hopefully they will help. Let me explain what the figure shows.

In my simulations, I use the average static pressure as the outlet boundary condition. When the outlet static pressure is set to 0.88 MPa, the calculated mass flow rate is 6.587 kg/s. When I change the outlet static pressure to 0.89 MPa, and use the solution at 0.88 MPa as the initial field, the situation shown in the figure occurs. It looks as if the calculation suddenly becomes “idealized”: the residuals drop sharply, the efficiency increases, and the behavior looks very strange. From the flow field, the separation vortex disappears and the flow becomes unrealistically ideal.

Additionally, I’d like to supplement my explanation with a case using a mass-flow outlet condition. Although this may not be the exact same impeller design as the one I mentioned earlier, the behavior is very similar, and I think it is still worth noting.
In this case, with a mass-flow outlet, I use the solution at a flow rate below the jump point as the initial field, and then compute a case above the jump point. Just as I described before, the residuals drop rapidly at the beginning, and the flow variables start converging toward seemingly reasonable values. However, at that moment, the residuals suddenly begin to rise gradually and then settle into a stable level. During this process, the efficiency deviates from the expected value and stabilizes at an abnormally low level.

[Opaque]

Thank you for posting those plots. Let me try to digest the information in the plots.

In the meantime, if you convert those mass flows to an "exit corrected mass flow" value using the proper reference conditions, and run the model using the Exit Corrected Mass Flow outlet option, what efficiency value will you get?

[ghorrocks]

This all seems to suggest to me that you have found a location where the turbulence model you are currently using suddenly jumps to predicting an incorrect flow field. My recommendations would be to try some different turbulence models to see if they are more accurate.

I would start by trying the options available on the SST model, such as curvature correction, SST reattachment modification and high lift modification.

If that does not help then you might have to go deeper and try the GEKO model, then SAS SST, DES or some of the LES options.

[LiuYD]

Originally Posted by Opaque

Thank you for posting those plots. Let me try to digest the information in the plots.

In the meantime, if you convert those mass flows to an "exit corrected mass flow" value using the proper reference conditions, and run the model using the Exit Corrected Mass Flow outlet option, what efficiency value will you get?

Thank you very much for your help!
I haven’t used the “exit corrected mass flow” boundary condition before. I checked the help documentation and some related posts in the forum, but I’m not completely sure whether I understand it correctly. It seems that this boundary condition is mainly used for operating points near surge, similar to the idea in compressor research where the actual inlet and outlet conditions in experiments are converted into design conditions.
I still need to study this part further. In fact, the compressor I am simulating uses an organic vapor working fluid, which is a non-ideal gas, so I am not yet sure how to apply this boundary condition or how to determine the reference temperature and pressure.
Still, it seems like a method worth trying, and I will experiment with it later.

[LiuYD]

Originally Posted by Opaque

Thank you for posting those plots. Let me try to digest the information in the plots.

In the meantime, if you convert those mass flows to an "exit corrected mass flow" value using the proper reference conditions, and run the model using the Exit Corrected Mass Flow outlet option, what efficiency value will you get?

In addition, I’ve noticed another phenomenon. When an impeller shows no abrupt transition in its performance curve, the results obtained using average static pressure at the outlet and mass-flow outlet boundary conditions almost completely overlap.

However, when a design does exhibit a sudden transition, the results from these two outlet boundary conditions become different, and the mass-flow value at which the jump occurs is also different.

So I would like to ask whether this indicates that there are some factors I haven’t considered yet.

[LiuYD]

Originally Posted by ghorrocks

This all seems to suggest to me that you have found a location where the turbulence model you are currently using suddenly jumps to predicting an incorrect flow field. My recommendations would be to try some different turbulence models to see if they are more accurate.

I would start by trying the options available on the SST model, such as curvature correction, SST reattachment modification and high lift modification.

If that does not help then you might have to go deeper and try the GEKO model, then SAS SST, DES or some of the LES options.

hello ghorrocks，your help is greatly appreciated!
I think this idea is very helpful. I have already tested several turbulence models, such as SST with curvature correction (SST-CC), the default GEKO model, and GEKO with an increased Separation Coefficient and curvature correction enabled. They have some effect—the location of the abrupt change shifts—but unfortunately the sudden transition still exists. I would like to attach a figure that shows the results obtained with different turbulence models.

I will also try some of the other models you mentioned, and I hope I can discover something useful.

[Opaque]

Originally Posted by LiuYD

Thank you very much for your help!
I haven’t used the “exit corrected mass flow” boundary condition before. I checked the help documentation and some related posts in the forum, but I’m not completely sure whether I understand it correctly. It seems that this boundary condition is mainly used for operating points near surge, similar to the idea in compressor research where the actual inlet and outlet conditions in experiments are converted into design conditions.
I still need to study this part further. In fact, the compressor I am simulating uses an organic vapor working fluid, which is a non-ideal gas, so I am not yet sure how to apply this boundary condition or how to determine the reference temperature and pressure.
Still, it seems like a method worth trying, and I will experiment with it later.

The exit corrected mass flow is a boundary condition intended for full range use, from choke to surge. That is not possible using a static pressure condition or a mass flow outlet condition.

Performance plots usually have distinct regions: high slope/vertical region -> choke, and small slope/horizontal region.

For each region, the setup is usually modified from a static pressure outlet BC to an outlet mass flow BC. The exit corrected mass flow is intended to run throughout the range w/o changing the model.

[ghorrocks]

If changing the turbulence model is moving the jump around then I suspect the turbulence model is the fundamental issue.

Don't forget to try the SST reattachment modification and high lift modification. They should be easy to try because the alternative approaches substantially increase the degree of difficulty.

If those SST modifications do not work then I suspect you are going to have to try a DES or LES approach. These are much harder to get working properly, but you might be entering a regime where it is required. The SAS and DES models are the first ones to consider as a full LES model is going to be very expensive.

[LiuYD]

Originally Posted by Opaque

The exit corrected mass flow is a boundary condition intended for full range use, from choke to surge. That is not possible using a static pressure condition or a mass flow outlet condition.

Performance plots usually have distinct regions: high slope/vertical region -> choke, and small slope/horizontal region.

For each region, the setup is usually modified from a static pressure outlet BC to an outlet mass flow BC. The exit corrected mass flow is intended to run throughout the range w/o changing the model.

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?

[LiuYD]

Originally Posted by ghorrocks

If changing the turbulence model is moving the jump around then I suspect the turbulence model is the fundamental issue.

Don't forget to try the SST reattachment modification and high lift modification. They should be easy to try because the alternative approaches substantially increase the degree of difficulty.

If those SST modifications do not work then I suspect you are going to have to try a DES or LES approach. These are much harder to get working properly, but you might be entering a regime where it is required. The SAS and DES models are the first ones to consider as a full LES model is going to be very expensive.

I also think the issue may be related to the turbulence model, especially when dealing with organic working fluids. I will try the SST reattachment modification and high-lift modification right away. Thank you again for the reminder.

[ghorrocks]

Are you operating in a region of your material properties where they are not too far from ideal gas (or incompressible)? Or are your properties strongly non-ideal (eg phase change)?

[LiuYD]

Originally Posted by ghorrocks

Are you operating in a region of your material properties where they are not too far from ideal gas (or incompressible)? Or are your properties strongly non-ideal (eg phase change)?

I think that under my design operating conditions, the organic vapor behaves much closer to a non-ideal gas. The relative Mach number inside the impeller can reach up to about 0.8, and the temperature is quite high, approaching the critical temperature. Although the pressure is still not very close to the critical pressure, overall I believe the fluid cannot be simplified as an ideal gas.

[ghorrocks]

I was not suggesting you could model this as an ideal gas. I was asking how far from an ideal gas is your conditions? In other words, non-ideal gas behaviour will create flow features which cannot exist in an ideal gas (phase change is one example), and these features will make the flow harder to converge and get accurate. If the non-ideal characteristics are a small contributor then you should be OK - but if they are strong this will complicate things.

You should also be aware that no turbulence model is tuned for accuracy in multiphase conditions, or non-ideal gas conditions. This is part of the reason I was asking - there is no turbulence model in existence which accurately models phase change flows or strongly non-ideal flows.

[LiuYD]

Originally Posted by ghorrocks

I was not suggesting you could model this as an ideal gas. I was asking how far from an ideal gas is your conditions? In other words, non-ideal gas behaviour will create flow features which cannot exist in an ideal gas (phase change is one example), and these features will make the flow harder to converge and get accurate. If the non-ideal characteristics are a small contributor then you should be OK - but if they are strong this will complicate things.

You should also be aware that no turbulence model is tuned for accuracy in multiphase conditions, or non-ideal gas conditions. This is part of the reason I was asking - there is no turbulence model in existence which accurately models phase change flows or strongly non-ideal flows.

I understand what you mean now, thank you! I checked the data, and under my conditions the compressibility factor is around 0.85–0.9, and although condensation is most likely to occur near the leading edge, I reviewed the parameters and confirmed that no phase change occurs. So I think it is reasonable to assume that the working fluid is non-ideal, but not severely so.

As for the turbulence model, I currently don’t have a good solution. After all, I can’t modify the model myself, and in many cases SST can already produce a reasonably normal performance curve (at least without the sudden jump). So this does seem to be a complicated issue with multiple factors involved. Thank you again for your help.