Large Errors in Propeller Efficiency vs Experimental Values

[giggy]

Hello,

I apologize in advance for the very long post

I am currently creating a study where I would like to predict the efficiency of an APC 11 x 5.5 propeller at constant RPM as the advance ratio increases. I then want to compare SimScale’s predictions with the measured UIUC data. My methodology is explained below:

I saw that SimScale already has a sample validation case with this specific propeller (Drone Propeller Study | Validation Case | SimScale), though this test is for static conditions only. Regardless, I used this exact project link as a starting point and copied it to my workspace.

I made the following changes from the settings that were originally in place for the static tests:

• Changed “Non Orthogonal Correctors” from 0 to 2 since the max Non-Orthogonality is 83.015 according to the meshing log (I am also surprised at the fact that the Non Orthogonal Correctors were set to 0 and not 2 in the SimScale static tests).

• Changed the inlet/outlet boundary conditions to “Velocity Inlet” (set in in/s calculated from advance ratio) and “Pressure Outlet” (0 gauge pressure)

• Changed the “Materials - Air” assignment to be assigned to just the flow volume (Part 2), it was previously assigned to both the MRF (part 1) and the flow volume (part 2). SimScale would not let me start the simulation when I first tried, and gave me this error: “In single region simulations, only the fluid region can be assigned to a material. Please review your material assignments, making sure that only the flow volume region is assigned.”

For all simulations I used “Mesh 3” which had y+ values of < 1 (according to the post processor) for the full resolution boundary conditions along with 3000 RPM (I initially did 6000 but it was no longer incompressible after checking the velocity magnitudes so only at simulation runs with “3000 RPM” in the title, the rest are 6000 RPM). After running several simulations at advance ratios that were listed by UIUC, and computing the efficiencies from the “Pressure Force Y” and “Pressure Moment Y” values. I came up with the attached graph and table.

I was quite surprised to see that the predicted efficiencies were very different from the UIUC data, especially since the static test data computed by SimScale in their validation case matched the UIUC data quite nicely. I was expecting to get values closer to the UIUC data, seeing as I was using the same propeller CAD model with the same refinements. This leaves me with the following immediate questions which I believe will help me solve my issue:

1. Why am I unable to start a simulation with air assigned to both the flow volume and MRF zone when it was done by SimScale already in their validation project (in Jan 2021 according to the simulation runs)

2. What effect would this have on the numerical accuracy of the simulation if any

3. Am I correct in saying that the y+ values for my simulations are good for the full resolution boundary condition given the fact that they are below 1?

4. Could the velocity inlet and pressure outlet boundary conditions be the culprits? Do I have to create velocity inlet and pressure outlet conditions where I specify turbulent kinetic energy and specific dissipation rate values?

5. Is there anything else I may be overlooking when setting up the simulation? The results all seem to converge.

PROJECT LINK: https://www.simscale.com/workbench/?pid=6220943220511267184&mi=run%3A103%2Csimulation%3A7&mt=SIMULATION_RUN

UIUC 3000 RPM Data: https://m-selig.ae.illinois.edu/props/volume-1/data/apce_11x5.5_kt0516_3010.txt

FINAL NOTE, I do not believe (or hope) that my calculations are wrong but I used the following:

Density: 1.196 kg/m3

n = 50 rev/s (3000 RPM / 60s)

D = 11 in (or 0.2794m since forces and moments are in N and N-m)

CT = Thrust / (Density * n^2 * D^4)

CQ = Torque / (Density * n^2 * D^5)

CP = 2 * pi * CQ

Efficiency = (CT/CP) * Advance Ratio

Thank you very much for your help and I apologize for such a long post but I wanted to explain my issue as clearly as I could.

[SBlock]

Hello giggy,

A very interesting project you have here.

Can you please try to simulate the case with the same boundary settings as provided in the validation case, because the increased velocity has an influence on the force and torque? This might explain when the difference increases with higher rpm’s as the rotor velocity differs more from the free stream velocity.

To your other questions.

1. I guess that this just has been changed for the current version of SimScale.
2. Which effect do you mean? In regards to the MRF not assigned to the Air region, this shouldn’t effect the Simulation since the MRF only changes the behavior if the cells within the MRF domain, which are also assigned to the Air volume.
3. Yes for full resolution BC the y+ value has to be very low since we don’t us a wall turbulence model to simulate the boundary layer. Therefore a lot of cells are required and also a very low +y value.
4. As stated in the top I would try to change the boundary condition to inlet-outlet boundaries so that air can exit/enter the fluid domain driven by the propellor.

I hope I could answer your questions.

Best reagrds
Sebastian

[giggy]

Hello SBlock,

I am confused, do you want me to copy the static boundary conditions from the validation case and make a simulation? Or do you want me to create a boundary condition with the same parameters and add a velocity component to it?

The first screenshot I have attached is the new boundary condition I have created and the lower screenshot is the boundary condition from the validation case

Thank you for your help.

[Retsam]

Hi @giggy.

It is not a direct answer to your problem, but I’ve just posted a very simplified setup of your propeller:

'Drone Propeller Again' simulation project by Retsam

I created a new simulation project called 'Drone Propeller Again': Small mesh and study of efficiency Minimal mesh and just two simulations to evaluate forces on a small propeller related to advance speed. More of my public projects can be found here. I used KISS approach to simulate the same propeller as Giggi (https://www.simscale.com/forum/t/large-errors-in-propeller-efficiency-vs-experimental-values/95004). It means that I spent <5% of resources and < %2 of time which was available for t…

Take a look: I see a good potential on your side and perhaps quicker pace in mesh / simulation would help.

Cheers,

Retsam

[giggy]

Hi @Retsam,

I took a look at your simplified simulation and ran it for my airspeeds and overall the results seem much better than before!

The efficiency curve better tracks the experimental one and also predicts maximum efficiency at the same points as the experimental data.

I was just wondering how did you create the cylindrical flow volume along with the frontal hemisphere? I seem to be able to only make rectangular flow volumes in SimScale’s “Edit in CAD mode” feature.

Thank you again for your help!

[Retsam]

I used OnShape for creation of my simulation domain, @giggy.

Due to low Reynolds numbers ( 30’000 ~ 60’000), I do not bother to use hyper low +y (<1). However mesh of propeller itself is really ‘coarse’ and will impact results. If you wish, you can play or tune my model and make better use of your core/hours trying to fit experimental results.

You will also find that my flow domain is small in respect to ‘orthodox’ knowledge of CFD. My rationale is that I do not create a simulation ‘tunnel’ with slip walls (as they need to be fare away from the model due to back pressure), but I used ‘Custom’ wall with all parameters set to ‘zero gradient’. That way simulation domain can be much smaller.

Take care and report on your interesting study (also on future ones), please!

Retsam

[SBlock]

Hi @giggy
I would use the bottom variation just to be sure that the velocity does not influence the results.
But when I take a look at the results you got from your setup and the setup from @Retsam , I would suggest that you do a mesh sensitivity study. With focus on the leading edge and the layer creation, since your mesh was over predictive and now you are und underneath your results.

Best regards Sebastian

[Retsam]

Good piece of advice, @SBlock.

Before making that sensitivity study I would go first to mesh log and spot ‘oddities’. They should be fixed. For instance my Mesh 1 log:

volumeRatio
Acceptable range: 0 to 1000
min: 1
max: 19988.726251687942

I did fix it in Mesh 2 by using Mesh > Advanced setting > Small feature suppression and setting it to 0.1 mm (0.0001 m).

Mesh 2 log:

volumeRatio
Acceptable range: 0 to 1000
min: 1
max: 12.537038040975991

This cleanup step brings not only better mesh but smaller mesh ( by about 25%) and smaller simulation times.

From that point on, you can think about better mesh for the propeller and follow Seb advice.

Cheers,

Retsam