[Julian121]

I would like to calculate the mass flow rates of recirculating flows in the attached 3D flow domain. The flow enters to the flow domain from right-hand side. Rotor is placed under this flow domain. Other than the two recirculating patterns, there is a recirculating flow that goes into the flow domain and leaves it from left-hand side. I followed the post on How to calculate mass of recirculation and defined a plane covering the recirculating flows, but I get very low flow rates which I think is not right. Is there another way to calculate such mass flow?

[ghorrocks]

There are many ways to calculate mass flow rates. But I have no idea what you are modelling or what you are trying to do so cannot suggest anything.

An obvious approach is to put a plane across the flow somewhere and calculate the mass flow rate through the plane. You say that gave unexpectedly low values - maybe you should explain what you did here and why you think it did not work.

[Gert-Jan]

You need to create a plane that covers only half the circulation. To obtain this, bound a full plane in X and Y dimension, such that it fits. Then calculate the massflow through this plane. Or integrate the normal velocity.
Alternatively with use of a full plane, define a new variable that clips (using a step function) the negative (=reverse) part of the velocity component normal through plane. Then integrate this velocity to get a volume flow.

[Julian121]

I am modelling a low-speed compressor in addition to a casing treatment (the flow domain in the first post) as unsteady. I am examining different configurations of the casing treatment in terms of stall margin improvement. In order to quantify the effectiveness of the casing treatment, I need to compare the recirculation mass flow between the casing treatment configurations. As the casing treatment is a 3D flow domain and there could be several recirculation flow patterns within it in x-y, x-z and y-z planes, I should consider the effects of these flow patterns somehow in an operating condition.

In addition to the recirculation within the casing treatment, there is a bigger recirculation, which is taking place between the rotor and the casing treatment. According to the literature this recirculation has more important effect. Can you please explain how to calculate this mass flow? Does it have similar procedure as the way of calculating the recirculation within the casing treatment? I was thinking I should apply the continuity equation to calculate the bigger recirculation, but I am not sure how to apply it.

[ghorrocks]

Thanks for explaining what you are trying to do, that puts things into context so we know what you are trying to do.

First of all, be aware of some fundamental mathematics - in 2D separations are clearly and uniquely defined by the separating streamline. There is, in general, no similar rule for 3D flows. There is no separating streamfunction in general. This means in 3D flow separations do not go around for ever (as they do in 2D), they have somewhere the flow gets in and somewhere the flow gets out. This means the fluid has only a finite time in the separation before it leaves and goes somewhere else.

The point of that comment is to say there is no unique and universal mathematical definition of separations in 3D flow. This means you have to make something up which is relevant to your flow, which captures what you perceive to be the separation.

If you define it as contained by a isosurface of zero velocity then you will find it is not closed (because of the flows in and out). But you may be able to cap it and that defines a volume.

If you are only interested on the size of the separation on a surface (eg what area of blade is covered by a separation) then looking at the wall shear stress is often useful. Where the wall shear stress reverses direction is a useful definition in many cases.

Other definitions include looking at the vorticity. Also have a look at the vortex core stuff in CFD-Post - that may be useful as well.

[Julian121]

To make it more clear what I mean by the recirculation between the rotor and the casing treatment, I attached an image. I would like to calculate the mass flow of the recirculation.

[ghorrocks]

Yes, I know what you want - but what I was saying is that it does not exist. There is no mathematical definition of recirculation size in 3D, and most recirculations in 3D are not true recirculations anyway (as they usually have a fluid in path and a fluid out path).

So my previous post said:
* There is no formal mathematical definition of recirculation in 3D, so you are going to have to make one up which looks good for your case.
* I suggested a few ways of doing this.

[Julian121]

Thank you for your explanation. Assuming I want this recirculation mass flow in 2D, where streamlines are clearly defined, CFD-Post does not show streamlines in both domains simultaneously since rotor blade has rotated (unsteady simulation) so I cannot visualize streamlines on a single plane containing rotor and casing treatment. I used graphical instancing feature to replicate both domains but a single plane on an axis cannot be created. What should I do?

[ghorrocks]

Note that taking a slice out of a 3D flow does not make it a 2D flow. The slice will have velocity components out of the plane which a true 2D streamline will not have. So it will not be strictly mathematically correct.

But having said that, it might be close enough to be useful. So it is worth considering.

I don't understand your comment about streamlines being created in both domains. Can you post an image of what you are getting?

[Julian121]

Please see the screenshot. Since the rotor has rotated, a plane including the rotor and casing treatment cannot be created. As a result, streamlines in both domains cannot be created.

[ghorrocks]

Can you use an Instance Transform on the rotor to copy the modelled section right around the circumference so there is always a continuous plane?

[Julian121]

I created the two planes as you said but there is some discontinuity between them. What should I do?

[Gert-Jan]

If this is what you created after using the Instance Transform. as suggested by Glenn, then your axis of rotation does not agree with the axis of rotation of your simulation. Alternatively, your axis of rotation in your simulation is incorrect.

[Julian121]

I managed to create a continuous plane including both domains! However, as the two planes are not necessarily coincident, the streamlines are not continuous at the interface between them. Shouldn’t the streamlines be continuous at the interface? I thought this is due to the relative motion between the rotor and the casing treatment, so I used “velocity in stationary frame”, but it did not change. Should I find the equation of the two planes that coincides to fix the problem?

[Opaque]

Have looked at the plot using only Forward, or only Backwards?

[Julian121]

The screenshots show the streamlines using just forward and backward options. Does it seem right? There is still discontinuity.