[Opaque]

Q: what is the source of the values you are trying to match?

Q: are they absolutely free of errors? Experimental data has error bands

are there other "fundamental checks" you can do that can increase the confidence on your results w/o having to look at someone else data?

Recall in practice, there will be no benchmark, and conclusions must drawn anyways. What kind of back of the envelope thought problems can be used to infere if the current data is valid or not?

[keg504]

Originally Posted by Opaque

Q: what is the source of the values you are trying to match?

Q: are they absolutely free of errors? Experimental data has error bands

are there other "fundamental checks" you can do that can increase the confidence on your results w/o having to look at someone else data?

Recall in practice, there will be no benchmark, and conclusions must drawn anyways. What kind of back of the envelope thought problems can be used to infere if the current data is valid or not?

The experimental data, though independent, I'm starting to realise is not the best quality. There are no error bands, as you say there should be. It's just some guy doing tests somewhere and uploading the data to a testing equipment manufacturer's website. (https://database.tytorobotics.com/te...-motor-ns22x66)
It will be verified somewhat soon though, in the university's wind tunnel. My simulation is a part of the larger project.

On a side-note, I made the flow compressible, and it is improving results a little, but not nearly enough to make up the difference.

Also, were those questions meant to be rhetorical?

[ghorrocks]

At Re=3E5 the flow is likely to be almost all turbulent for most airfoil shapes - unless this is a laminar flow airfoil. That means using a turbulence model for the entire this is likely to be OK (again, unless it is a laminar flow airfoil).

Propellers often have separations near the hub as the blade is often quite fat in that region. This usually does not make much of a difference the blade near the hub does not contribute much to propeller performance.

To visualise the separations you will want to look at the wall shear on the blades. Where it goes to zero or reverses direction you have a separation.

[Opaque]

Originally Posted by keg504

Also, were those questions meant to be rhetorical?

Not at all. I used to teach, and I would have likely asked you similar questions as you were making progress in your project.

The idea here is to help you find the solution by yourself and help solidify your modeling skills. You are making great progress.

[keg504]

Hi Glen, I've plotted the wall shear. It looks like the flow separates at a similar location for all rotational speeds, near the leading edge of the propeller. For almost all RPM values, the load distribution seems to be the same, with the highest pressures concentrated at the leading edge, and dropping off very quickly after that. Is there a way to tell whether the propeller is meant to be laminar or turbulent?

I can see that the contour plots show irregularities in the blade profile, so it seems most likely that my CAD model is the culprit here.

Moving on to contra rotating coaxial rotors, would it still be acceptable to use frozen rotor as the interface between the rotors? From my understanding, FR is highly dependent on the rotor position, but I want a more general idea of the performance. Would I use a periodic interface, or stage, then?

edit: I read up a bit more about pitch, so seems that mixing planes is not suitable at all.

Here are the shear plots:
2273 RPM
2273_wall_shear.png

3727 RPM
3727_wall_shear.png

4471 RPM
4471_wall_shear.png

[Opaque]

Originally Posted by keg504

Hi Glen, I've plotted the wall shear. It looks like the flow separates at a similar location for all rotational speeds, near the leading edge of the propeller. For almost all RPM values, the load distribution seems to be the same, with the highest pressures concentrated at the leading edge, and dropping off very quickly after that. Is there a way to tell whether the propeller is meant to be laminar or turbulent?

I can see that the contour plots show irregularities in the blade profile, so it seems most likely that my CAD model is the culprit here.

Moving on to contra rotating coaxial rotors, would it still be acceptable to use frozen rotor as the interface between the rotors? From my understanding, FR is highly dependent on the rotor position, but I want a more general idea of the performance. Would I use a periodic interface, or stage, then?

edit: I read up a bit more about pitch, so seems that mixing planes is not suitable at all.

Here are the shear plots:
2273 RPM
Attachment 99833

3727 RPM
Attachment 99834

4471 RPM
Attachment 99835

The interface between counter-rotating rotors should be either a "transient rotor-stator sliding interface" for a transient simulation, or a "mixing plane" for a steady-state simulation.

[ghorrocks]

No - you are looking at the wrong wall shear.

If the flow is attached the wall shear will be in the direction of flow of the air over the surface. If the flow is separated it will be against the direction of the bulk air flow. So the wall shear direction you should be looking at is y direction on your images in post #45.

You showed the Z direction which is not very meaningful for observing separations.

Even better, draw vectors on the blade surface of wall shear using the X, Y and Z components. That should really clearly show any separation as a reversal of the wall shear. This approach has the advantage of working no matter the surface curvature is or the orientation of the blade. Looking at the Wall Shear Y component will only work in the current position of the blades.

[keg504]

I did plot x and y shear contours, they both looked mostly negative, so I didn't think they were useful. But here are the shear vectors. I'm not quite sure how to interpret them, but it looks like the flow remains attached for the most part.

2273 RPM
2273_wall_shear_vect.png

3737 RPM
3727_wall_shear_vect.png

4471 RPM
4471_wall_shear_vect.png

[ghorrocks]

The recirculations are usually a much lower velocity than the main flow. So you will have to scale the vector length up so you can see what is happening in the low flow regions.

The reason I ask this is because attached flows can be predicted quite accurately with normal turbulence models, but separated flows often require a more sophistocated model to get high accuracy. So working out whether you have significant separated regions determines which approach you need to look at.

[keg504]

I scaled up the vectors to be as large as they would go in CFD-Post. Here are the results. It looks like the flows do remain attached, except near the hub, as you stated.

2273 RPM
2273_wall_shear_vect.png

3727 RPM
3727_wall_shear_vect.png

4471 RPM
4471_wall_shear_vect.png

[ghorrocks]

Yes, that does look like there are no separations. That makes things considerably easier - it means a normal 2 equation turbulence model should be quite accurate.

[keg504]

So I've been running simulations of the co-axial configuration. I've noticed a discontinuity in pressure across the mixing plane interface (I'm using stage average velocity with implicit averaging). Is that something to be worried about? The total pressure and velocity seem to remain continuous.

Also, I'm pretty sure the geometry is the problem in my case. I've been running a 60 in propeller that I have the manufacturer CAD for, and even without a proper mesh study (I'm using a similar number of elements), the difference is only ~3% under.

Here you can see the total pressure and pressure plots for the coaxial simulation (the blank space in the middle is meant to represent the motor, it is a cylinder):

Total pressure
3429_coax_final_tot_press.png

Pressure
3429_coax_final_press.png

[Opaque]

Originally Posted by keg504

So I've been running simulations of the co-axial configuration. I've noticed a discontinuity in pressure across the mixing plane interface (I'm using stage average velocity with implicit averaging). Is that something to be worried about? The total pressure and velocity seem to remain continuous.

Also, I'm pretty sure the geometry is the problem in my case. I've been running a 60 in propeller that I have the manufacturer CAD for, and even without a proper mesh study (I'm using a similar number of elements), the difference is only ~3% under.

Here you can see the total pressure and pressure plots for the coaxial simulation (the blank space in the middle is meant to represent the motor, it is a cylinder):

Total pressure
Attachment 99916

Pressure
Attachment 99915

May I ask why the "stage average velocity" option for the mixing plane instead of the default option?

[keg504]

My reasoning is that even though I have turned on compressible flow, the flow isn't actually at Mach 0.3, so constant total pressure would compromise on the simulation if one of the two has to be reduced in relation to the other to maintain it. I do have it in mind to test with the other option, but time is not on my side right now.

I'm aware that the reasoning is incomplete and probably misunderstanding something, but I couldn't find a reference on which option to choose.

edit: also, I was basing it on blade element theory, namely I'm attempting to approximate propeller velocity by using the stage average velocity

[Opaque]

Originally Posted by keg504

My reasoning is that even though I have turned on compressible flow, the flow isn't actually at Mach 0.3, so constant total pressure would compromise on the simulation if one of the two has to be reduced in relation to the other to maintain it. I do have it in mind to test with the other option, but time is not on my side right now.

I'm aware that the reasoning is incomplete and probably misunderstanding something, but I couldn't find a reference on which option to choose.

edit: also, I was basing it on blade element theory, namely I'm attempting to approximate propeller velocity by using the stage average velocity

The default is there for a reason: to minimize user error by making uninformed decisions.

The old default, pre-Ansys CFX-18R1 used to be stage average velocity and it was superseded by a more accurate model.

Total pressure behavior should be irrelevant to compressible or incompressible fluid. If it were dependent on that difference, it would be a big problem since a user would need to know when to blend the models, i.e. which parameter determines which model to use.

[keg504]

Thanks for the clearing that up. I hope I have time to change it, but probably not right now, so I will use as-is for now.

Would you be so kind as to explain the actual difference between stage average velocity and constant total pressure, so that I know for future reference, please?

[keg504]

I changed it to constant total pressure, as you suggest, Opaque, and it helped a little, but not drastically, though I don't think it would, just would stand up more to scrutiny.

I think my problem has been largely solved, thank you ghorrocks and opaque for your help and patience. There might be optimisations that can be done, I'm not too worried though.

As a summary for those might setup a similar case here it is:

For a steady state simulation of static propeller thrust in an outdoor environment, use a stationary outer domain with air as an ideal gas, with an inlet set to an opening condition, and outlets set to also be opening. All openings have a reference pressure of 0. The inlet and outlet should be separate, otherwise the imbalances will not converge. The size of the air domain used is 8 * rotor diameter. The reference pressure is 1 atm. Compressible flow is also turned on.

The rotor domain is rotating, using a frozen rotor interface with the air, and a mixing plane interface (using constant total pressure) with the other rotor. The rotor diameter used is a cylinder with diameter 1.1 * rotor diameter and a length of 0.4 * rotor diameter (the length can vary based on rotor spacing in the coaxial configuration).

The domain dimensions come from "3D CFD Simulation and Experimental Validation of Small APC Slow Flyer Propeller Blade" (Kutty and Rajendran, 2017).

If I've missed anything, let me know, and I'll edit this post .

[keg504]

The test rig for the coaxial configuration has been mostly set-up, save for automated data collection, but preliminary testing using multimeters and hand held stroboscopes are showing that my simulations roughly match the experimental data after the aforementioned nebulous adjustment factor. Better data will be collected, but right now, I would say the error is about 10%.