[keg504]

Hi,
I'm trying to do a simple propeller simulation based on this paper: 3D CFD Simulation and Experimental Validation of Small APC Slow Flyer Propeller Blade (Kutty and Rajendran, 2017), using a different 22 in propeller from T-motor. I've set up a simulation using both Frozen Rotor and Mixing Planes in CFX, and tried a few different Boundary Conditions: inlet: velocity, mass flow and total pressure, outlet: avg. static pressure, static pressure, opening), conducted a mesh independence study, and none of these seem to match the experimental thrust. (Mixing planes always ends up with floating point overflow, even with double precision). Right now, I'm trying a physical timescale of 1/propeller rotational velocity (rad s-1). I have been using the k-omega SST model.

What I am trying to do is a static thrust study of the propeller. Can someone point me to to a paper or resources on how to set this up correctly, or explain the appropriate boundary conditions? I've been stuck on this issue for a month, and I'll need to move to a co-axial co-rotating study once this is done, so I want to get this right and understand why before moving on. An issue I'm seeing is that the velocity leaks radially instead of through the propeller. Hopefully I've attached the images correctly.
438065022_960348448716476_6737782057466766531_n.jpg

438065217_1645858406189039_5850337538447370833_n.png

438083337_1359463431392043_2573848191980117877_n.png

438051586_884524410101071_5336072679999309056_n.png

[ghorrocks]

What are you trying to model? What results do you want to see (I think you said you want static thrust)? What conditions is this running at (ambient velocity, atmospheric conditions, surrounding fluid, rotor speed etc)?

What conditions is this fan designed to run at?

[keg504]

Apologies, I overlooked adding those details. This is the experimental data I am trying to model: https://database.tytorobotics.com/te...-motor-ns22x66

Essentially, this is for a drone propeller at hover conditions at sea level at ambient velocity (assuming still air for now). I was trying to run it at the highest thrust (4471 RPM). This is supposed to be in open air. I'm not sure what other details you need, but I'll try to tell you if I know them.

I also got a floating point error just now for mixing planes for the physical timescale I mentioned of 1/propeller rotational velocity (rad s-1).

[ghorrocks]

How many blades does the propeller have?

[keg504]

Two blades, I am using half domain symmetry on the domains though.

[Opaque]

Originally Posted by keg504

Two blades, I am using half domain symmetry on the domains though.

Be careful with the vocabulary here. Are you using Symmetry or a Domain Interface with Option = Rotational Periodicity?

In Ansys CFX, Symmetry is planar and represents a mirror condition.

[keg504]

Originally Posted by Opaque

Be careful with the vocabulary here. Are you using Symmetry or a Domain Interface with Option = Rotational Periodicity?

In Ansys CFX, Symmetry is planar and represents a mirror condition.

It is a symmetry boundary condition, I am only simulating one blade to reduce computational time.

[ghorrocks]

You are using the wrong boundary condition. You should be using rotational periodicity on both the rotor domain and the ambient domain. Your incorrect use of a symmetry boundary condition is one of the reasons why the results are weird.

Have a look at the rotating machinery tutorial examples for CFX to see how rotating machinery simulations should be set up.

[keg504]

Ok, I didn't realise, I will take a look at it and report back once I've run a simulation. I presume this tutorial is within ANSYS CFX's help?

Thank you!

[Opaque]

Originally Posted by keg504

Ok, I didn't realise, I will take a look at it and report back once I've run a simulation. I presume this tutorial is within ANSYS CFX's help?

Thank you!

In CFD modeling, in particular turbomachinery, the word Symmetry is used for Cartesian symmetry/mirror symmetry, and Periodicity is used for repetitive symmetry be it translational or rotational.

In Ansys CFX, symmetry enforces no flow crossing, i.e. V dot N == 0. That is not a valid BC for modeling a reduced "repetitive model"

In structural modeling, the wording is a bit different: rotational symmetry, or cyclic symmetry (time and space).

I would not be surprised, other vocabulary is used in other fields as well.

Summary: vocabulary is EXTREMELY important.

[ghorrocks]

You can access the tutorials on the ANSYS Customer page. For academic customers I think it is on the ANSYS academic site as well, but I have not checked.

You can also do a google search for "CFX turbomachinery tutorial" and you will find lots of them.

[keg504]

So I ran a simulation based on the periodic boundary, and I'm pretty sure that the inlet boundary condition is wrong (I used an absolute pressure of 1 atm), and you can see the results below. This is still with FR.
periodic_plane.jpg
Is it that the velocity inlet is correct for static thrust? I did ask a professor at my university, and he told me that wind tunnel conditions should be used, which has a stagnation inlet. In that case, does it mean that the dynamic pressure for the stagnation pressure is calculated using the expected exit velocity for the thrust based on momentum theory? (I used this reference: https://www.grc.nasa.gov/WWW/k-12/airplane/propth.html)

[ghorrocks]

I would set a reference pressure of 1 atm, and make all outer boundaries an opening at 0 Pa. The rotor and ambient domains have the rotational periodicity interfaces, of course.

[keg504]

Currently running a simulation, will take a day more to get results, here are the residuals so far.
First for frozen rotor:
Residuals_518_FR.png
Next for mixing planes:
Residuals_537_MP.png

[ghorrocks]

Why keep running it? It converged as tight as it is able at about iteration 50 and everything beyond that is a waste of time. See this FAQ: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

[keg504]

I was waiting for the turbulence residuals, since those seemed to be on a downward trend when I checked yesterday, but they were also oscillating now. Here are the pressure distribution results, and as you can see, there is little improvement. I will try running it without the periodic boundary, instead with the whole rotor to simplify it a bit, since it's converging quickly anyway.
Here are the mixing planes results, which got a thrust of 1469.27 N (it's supposed to be around 45 N)
MP_press.png
And here it is for the frozen rotor (thrust of 1205.39 N, for same conditions)
FR_press.png

[ghorrocks]

Your thrust is a long way off what it is meant to be, so something is seriously wrong with your simulation.

Please read the documentation about the GGI interface models - frozen rotor, mixing plane and the others. I think you will find the mixing plane model is not appropriate for what you are trying to do.

Please post an image of the mesh near your blades, the flow near your blades and your output file. You can trim the output file down to the first 50 iterations if you like. Please post it directly on the forum, do not use third party sites.

[keg504]

Hi,

Thanks for the help so far. Please see the mesh, flow and outfile attached. I'm not sure if this is what you were asking for in terms of the flow near the blade, it is taken from the centre point of the blade. If you need better images, let me know what kind. The forum seems to have blocked me from connecting because I messed up with the attachements earlier
Mesh
blade_mesh_small.png
Pressure around blade
blade_pressure.png
Velocity around blade
blade_velocity.png
Outfile
FR_100.txt

I have noticed that double precision is off even though I have set it to on in the bash script as follows:

#!/usr/bin/env bash

#SBATCH -A C3SE2024-1-15 -p vera
#SBATCH -J UAV_thesis
#SBATCH -n 32
#SBATCH -t 2-12:00:00
#SBATCH --mail-user=gnanaraj[at]chalmers
#SBATCH --mail-type=BEGIN,END,FAIL

#SBATCH -o out.stdout
#SBATCH -e err.stderr


module load ANSYS/2021R1

nodes="sed -e :a -e N -e 's/\n/,/' -e ta $TMPDIR/mpichnodes"
/apps/Common/software/ANSYS/2021R1/v211/CFX/bin/cfx5solve -def CFX.def

-par -par-dist $nodes -start-method "HP MPI Distributed Parallel" -double

#end of script (make sure line before this gets run)

The reason I am using mixing planes as well is because I want to run the propellers in a co-axial contra-rotating configuration after I have validated this. The CFD Online wiki suggests that mixing planes would be better because in frozen rotor, the blades are fixed in place, and flow is dependent on the relative positions, so I thought that it would be a more valid comparison for my report if the same interface was used for both simulation types.

[ghorrocks]

I see lots of problems in your output file:
1) Your inlet is 1atm and your outlets are 0atm! This is going to create a cyclone from the inlet to the outlet. Is this what you intended? I would expect that all external boundaries should be set to 0atm pressure.
2) Your reference pressure is 0 atm. If this device operates at normal atmospheric conditions then use a reference pressure of 1 atm. This reduces round off errors.
3) You probably want to use double precision numerics. It is easy to implement and can help so you might as well.
4) There are warnings saying you cannot use pitch change specified by angles and you should use option = None. I would implement this advice.
5) You have 4 interfaces. Why so many? Also, some of them are showing high non-overlap areas fractions. This suggests some of your interfaces are not connecting properly.
6) Your convergence is poor. Read the FAQ I linked to in my previous post. Also the things I have mentioned here will also help convergence.

[keg504]

1&2 - Ok, points 1 and 2 were completely my bad, I misunderstood the boundaries and pressures you mentioned.
3 - I have turned it on now, since I put the flag in the wrong location
4 - I used the suggested pitch change of None
5 - I combined the FR interfaces to 1 (I didn't realise you could select multiple locations)

I am running a simulation with these changes, and adjustments to improve convergence. Fingers crossed that this works!