[Julian121]

I have followed the instructions about using large time scale and coarse mesh in the region where instability exists, but nothing changed. The important parameters such as mass flow or pressure ratio still fluctuate.

In my case there exist some flow recirculation and separation from the suction side of a stator.
I still have doubts about this problem even though I have worked on it for months!


Glenn, may I send it to you?
I would be very grateful if you could look at my files.

[ghorrocks]

I don't have time to look at people's files in detail.

If you read the FAQ: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

It says that if the normal tricks to get it to converge fail then your only option is to run it transient.

[Julian121]

Following the previous simulations, I run some new simulations with updated mesh.

The operating point is close to the last measured data (stall point) in experimental results.

I have noticed that the mass flow in the inlet and the pressure ratio are oscillating. Is this a sign of stall or it is due to some numerical reasons? If this is a sign that stall or surge is present, according to the experimental results stall should occur at less mass flows.

Imbalances are not good either.

What do you think I should do?

[ghorrocks]

The oscillating pressure ratio is a sign the flow is moving, and therefore it is a transient flow, not steady state. These become more common as you approach stall or other off-design flow conditions. Whether this is important depends on how accurate you need your results - the results you have may be of sufficient accuracy depending on your requirements.

If you require a more accurate simulation then the only way forward is likely to be a transient simulation. This will be a much more expensive simulation, but it the only way to get some tricky flows to converge.

This is all explained in the FAQ I linked to.

[Julian121]

Originally Posted by ghorrocks

The oscillating pressure ratio is a sign the flow is moving, and therefore it is a transient flow, not steady state. These become more common as you approach stall or other off-design flow conditions. Whether this is important depends on how accurate you need your results - the results you have may be of sufficient accuracy depending on your requirements.

If you require a more accurate simulation then the only way forward is likely to be a transient simulation. This will be a much more expensive simulation, but it the only way to get some tricky flows to converge.

This is all explained in the FAQ I linked to.

Following the difficulty I had faced to obtain convergence in the steady simulations, I decided to run transient simulations to see if the convergence improves. However, when I was doing the transient simulations, some information about non-overlap area was reported with every time step.

Then, I performed a sensitivity analysis and it seemed that it had no effect. Now, I am inspecting my steady setups again and I found out that the non-overlapping area do exist in the steady problem too.

I am not sure whether this issue prevented me to obtain convergence in steady simulations but I think I should fix it. The non-overlap amount is on the order of 1e-2.

The interface is located between the Rotor and the CT.

How can I find the location of this area?
Does CFX treat it like a wall boundary?
Could you advise me on how to fix it?

Domain Interface Name : CT Per

Discretization type = GGI
Intersection type = Restarted
Non-overlap area fraction on side 1 = 9.02E-05
Non-overlap area fraction on side 2 = 6.46E-05

Domain Interface Name : CT to Rotor

Discretization type = GGI
Intersection type = Restarted
Non-overlap area fraction on side 1 = 1.75E-05
Non-overlap area fraction on side 2 = 4.58E-02
Pitch ratio ( pitch side 1 / pitch side 2 ) = 0.950
Pitch angle for side 1 [degrees] = 9.000
Pitch angle for side 2 [degrees] = 9.474

[Opaque]

Have you looked in the post-processor for the "Nonoverlap Fraction" in the variables list?

[Julian121]

Originally Posted by Opaque

Have you looked in the post-processor for the "Nonoverlap Fraction" in the variables list?

It seems that the area under the vanes are in the non-overlap portion of the Rotor/CT interface.

The vanes have been removed from the CT domain.

Should I change the rotor domain?

Do you think this may cause any difficulty in steady state simulation?

[Opaque]

The non-overlap portion is treated as a wall.

Is the non-overlap portion sliding when running in transient? If it does, you have another frequency exciting the system.

Since you have not been able to obtain a steady periodic solution, you must reduce your model to something you can obtain what you expect first before increasing the complexity.

[Julian121]

Originally Posted by Opaque

The non-overlap portion is treated as a wall.

Is the non-overlap portion sliding when running in transient? If it does, you have another frequency exciting the system.

Since you have not been able to obtain a steady periodic solution, you must reduce your model to something you can obtain what you expect first before increasing the complexity.

Yes, it is moving as the rotor rotates. I loaded the results at different time steps and the non-overlap area do exist.

Does this area affect the results? This area is beneath of the vanes and flow cannot cross the vanes.

This model is a simpler model of a more complicated model. In the original model, the vanes have been extended and they come to the rotor domain.

I have done few steady simulations for this model too but even there steady convergence was not possible below 1e-4. I have attached some images of non-overlap fraction variable for this model.

It seems that no obstacle is placed in the flow direction for this model.

I can raise the vanes so they do not collide with the Rotor/CT interface in the modified model. Does it help?

Shall I continue the transient run?

[Opaque]

Got it. The non-overlap region is the hollow part of the vane. Since there is no chance the flow ever crosses that region, it should be fine.

I would continue the transient run at least to a full turn, i.e. the rotated pitch >= 360 [deg]