[keg504]

I've run a simulation with a coarse mesh (i.e. ANSYS mesher default settings) and I got the following results. The convergence, as you can see, isn't that great, I think the mesh is probably the main issue with that. The thrust is within line of what I expect, but I think better convergence based on the wiki will get a clearer picture, but the pressure and velocity plots are looking quite good!

Blade pressure:


Domain pressure:


Domain total pressure:


Domain velocity:


Domain velocity in z:


Velocity streams:


Mass and momentum residuals:


Imbalances:


Turbulence residuals:


Force on blade in z:

[Opaque]

It seems the simulation is converging nicely, but a bit slow for me.

Perhaps you should increase the physical timescale a bit. Are you using Auto Timescale, or Physical Timescale? Check the diagnostics for the Linear Solver section of the output file (read documentation) for the P-Mass equation, and H-Energy? What values do you see? @9.x or @5.x?

If 5.x, increase the timescale by a factor 5. If 9.x, about factor of 2, not too much.

[keg504]

I ran a finer mesh, and the convergence was worse. I was using auto-timescale, which was using a factor of 1.

I am running a simulation (or it's in queue, anyway) with a physical timescale of 1/rotational speed [rad s-1] to check the effect on convergence.

I can set it up to use a factor of 5.x and 9.x if that would be better?

[Opaque]

Originally Posted by keg504

I ran a finer mesh, and the convergence was worse. I was using auto-timescale, which was using a factor of 1.

I am running a simulation (or it's in queue, anyway) with a physical timescale of 1/rotational speed [rad s-1] to check the effect on convergence.

I can set it up to use a factor of 5.x and 9.x if that would be better?

As I said, check linear solver diagnostics. Without such information, it would be guessing.

[ghorrocks]

The coarse mesh simulation is converging nicely, as opaque states. You can see the jet from the fan has not reached the exit boundary yet - that is why the imbalances are still bad. Once the jet reaches the boundary it will start converging more quickly.

I adjust the physical time step size a bit differently to opaque. I start the simulation (often with the default time step like you have), and once it is starting to converge I use ëdit run in progress" to increase the time step by a factor of 2x - 10x. Watch the convergence for the next 20 or 30 iterations, and if it is still converging smoothly you can consider increasing the time step size again, but if it does not like it (either diverging or wobbly convergence) then make the time step size smaller. This way you can manually find a reasonable time step size for your simulation. Note that you almost always can converge a lot faster than the defaul time step size.

[keg504]

I've run with new timestep settings. Using a pyhsical timestep of 1/rotational speed [rad s-1] gives a value of 5.x, similar to an auto timescale of 10, which completes in about 600 iterations. If I set it to 15, then completes in about 420 iterations, still with 5.x.
I also ran a finer mesh for the physical timestep, and got about 600 iterations. The jet does reach the boundary with the finer mesh, but the thrust is lower (~37 N for finer mesh, ~39 N for the coarse mesh). What exactly should I be using as a metric for grid independence then, because if I compare the difference in simulated thrust to experimental thrust, the finer meshes are worse, counterintuitively, even though I hesistantly say they are more accurate (from my limited understanding), even if I use coefficient of thrust?
You can see the results here:
Larger timesteps, coarse grid:





Larger timesteps, finer grid:

[ghorrocks]

Your simulation is not converged if the jet has not reached the exit boundary yet. If the residuals are converged before the jet gets to the exit boundary then I would add imbalances to the convergence criteria, as they should pick up on this problem.

There is no point doing a mesh sensitivity study on simulations which are not converged. So get reliable convergence first and then do the mesh sensitivity.

[keg504]

For clarification, which boundary do you mean? The air in front or behind of the propeller? I set a conservation target of 0.01 and it didn't converge even after 10000 iterations. Should I move the boundaries closer to the propeller? From the velocity streams, you can clearly see that air is being pulled from the front of the propeller from the boundary. The imbalances don't make physical sense either, since the air is being pushed out of the boundary, according to the pressure and velocity plots (ignoring the streamlines for now). This would suggest a negative imbalance, no? You can see the results here:
Mass imbalances:

Thrust monitor:

Velocity streams:

Velocity plot:

Pressure plot:

Total pressure plot:

[ghorrocks]

My comment about the exit jet reaching the boundary was referring to post #21. Your post #26 shows the jet reaching the boundary which is good.

You will want to get your imbalances down to under 1% if possible.

But in your case I suspect you have the entire outside face as a single opening boundary. Is this correct? If you do this you will never get your imbalances to converge as there will always be some small numerical noise in the total flow over the face (let's call if A), but if there is only one face then the imbalances are approximately this flow A divided by the total imbalance which is also about A, meaning that your imbalance will be about 100%.

To fix this, split your outer boundary into an upstream boundary and a downstream boundary. They can still be openings, but you will now have a net flow on each boundary and the imbalance calculation will give meaningful numbers.

Your thrust graph showed it converged long ago. So I suspect you will find if you correct this imbalance issue it will declare convergence when the thrust levels out.

[keg504]

Originally Posted by ghorrocks

My comment about the exit jet reaching the boundary was referring to post #21. Your post #26 shows the jet reaching the boundary which is good.

You will want to get your imbalances down to under 1% if possible.

But in your case I suspect you have the entire outside face as a single opening boundary. Is this correct? If you do this you will never get your imbalances to converge as there will always be some small numerical noise in the total flow over the face (let's call if A), but if there is only one face then the imbalances are approximately this flow A divided by the total imbalance which is also about A, meaning that your imbalance will be about 100%.

To fix this, split your outer boundary into an upstream boundary and a downstream boundary. They can still be openings, but you will now have a net flow on each boundary and the imbalance calculation will give meaningful numbers.

Your thrust graph showed it converged long ago. So I suspect you will find if you correct this imbalance issue it will declare convergence when the thrust levels out.

Your suspicion was spot on, I thought it could be the case, but dismissive since it didn't make sense why it would matter, but your explanation clarifies it for me .

Results:



I suppose now is the time to move to the independence study. Are there resources for how to size grids for stationary and rotating domains? I know that a general rule is that closer to the propeller surface the grid needs to be finer, and to take into account boundary layer effects, and that inflation can be useful. But what I'm struggling with is how to decide when is good enough for one domain before adjusting the other. Is there a way to test multiple domain meshes at once using the same simulation, or do they all need to be run separately? Same with RPM tests, is there a method?

[Opaque]

Since a propeller sees mostly axial flow, and you are using a rotating domain, you should set the Alternate Rotation Model = On

It minimizes discretization errors.

[ghorrocks]

For the mesh independence study you can either:
1) Do it section by section, and optimise the mesh for each section as you describe, OR
2) Refine the mesh everywhere by the same ratio, so you do everywhere at once. So every mesh length parameter from the bulk mesh to the boundary layer is halved at the same time.

I rarely have time for 1, so I usually do 2.

Note that each comparison in the mesh refinement study should have the element edge length (not volume) changed by a factor of around 2. This means that a mesh with N elements will have 5N to 8N elements after refining. You need a significant change in the mesh density for mesh sensitivity studies to work.

[keg504]

I've been running the grid study, and it was going pretty well when refining the air mesh. However, when I'm refining the propeller mesh, the thrust drops by ~3 N. I've only done 1 refinement (the next one is struggling to mesh and I'm figuring it out right now.) What should I be using as a criteria if the target criteria is not working as a metric to define the mesh independence? Or am I misunderstanding it and the amount of change is what actually matters, which I'm starting to belive is really the point of mesh independence studies?

Here are my results so far:
mesh study.png

[ghorrocks]

For an accurate CFD model, you need:
1) An accurate mathematical model of the physics
2) An accurate numerical solution of the mathematical model.

A mesh sensitivity study only checks (2). If your results are wrong after you have good mesh independence (and convergence, and time step independence if transient) then (1) is wrong.

In your case things like upstream boundary conditions (for example turbulence conditions), surface roughness and turbulence model choice can make subtle differences which you need to get right to get those last few % accuracy.

The results you have done so far are looking internally consistent and monotonic. A more sophisticated way of doing mesh independence is by using Richardson extrapolation. I suspect it would work well in your case. It allows you to predict the mesh independent result without having to do the very finest meshes. Feel free to give it a go if you feel brave.

[keg504]

I managed to run a new finer propeller mesh, and it seems that the results are getting worse. I don't have the computing resources to go even finer to investigate, especially since the results file will be very large (the last one was already 16 GB), and I only get 30 GB on the cluster. Can I say that the mesh study is done for the propeller? How would I justify that given the regressive data? I can see that the air domain mesh study is done, due to small changes between mesh refinement.

You can see the result here:
mesh study.png

[Opaque]

Originally Posted by keg504

I managed to run a new finer propeller mesh, and it seems that the results are getting worse. I don't have the computing resources to go even finer to investigate, especially since the results file will be very large (the last one was already 16 GB), and I only get 30 GB on the cluster. Can I say that the mesh study is done for the propeller? How would I justify that given the regressive data? I can see that the air domain mesh study is done, due to small changes between mesh refinement.

You can see the result here:
Attachment 99741

You cannot define the mesh independent study on a single component having it sharing a frame change interface with another component.

The accuracy of the interaction across the frame change interface is a function of the mesh quality on both sides. Refining one side would introduce errors because the change in aspect ratio, and circumferential mesh quality.

[keg504]

Originally Posted by ghorrocks

For the mesh independence study you can either:
1) Do it section by section, and optimise the mesh for each section as you describe, OR
2) Refine the mesh everywhere by the same ratio, so you do everywhere at once. So every mesh length parameter from the bulk mesh to the boundary layer is halved at the same time.

I rarely have time for 1, so I usually do 2.

Note that each comparison in the mesh refinement study should have the element edge length (not volume) changed by a factor of around 2. This means that a mesh with N elements will have 5N to 8N elements after refining. You need a significant change in the mesh density for mesh sensitivity studies to work.

I was doing it as described in (1), I suppose that the way I did it is not the same as ghorrocks means? If that is the case, can you explain what section by section means here?

[keg504]

I ran the simulations using the best grid I have, and I'm getting a systematic error of at least 15%, decreasing as the RPM gets lower. It's around 5% at 1606 RPM, but the next point at 2273 after is ~16%. I tried adding a velocity inlet since I thought that could be the problem, but that made it worse as velocity went up, but based on BEMT that makes sense. Setting a mass flow rate at the frozen rotor interface, also based on BEMT helps, but very little. There's something missing in the setup, does anyone have an idea?
Based on this paper: https://www.mdpi.com/2504-446X/4/3/42, CFD using k-omega is getting similar results, and they apply a correction based on the airfoil lift and drag coefficients. They are using OpenFOAM. They got a factor of 1.7 for coefficients. If I apply a factor of about 1.2, I get similar results to the experiment. It still starts diverging at higher RPM.

Is it the airfoil shape that would then be the issue in my case? I do not have the manufacturer CAD either, so I used a point cloud scan to draw airfoil profiles and generate a rotor model in CAD. Is that the main issue? I did not guess the airfoil as they seem to have done in the paper.

You can see the results of the RPM variation here.
Thrust:
thrust.jpg

Coefficient of Thrust Ct:
Ct.jpg

[ghorrocks]

As the rotation speed increases the boundary layers will get thinner and the flow more turbulent (at least in the trailing section of the foil), and the turbulence transition point will move closer to the front of the foil. This means the turbulent flow section becomes increasingly important and the laminar section less important.

What is the airfoil Re number? Do you know where the turbulence transition point is? Do you know whether there is an separations or stall?

Also - if the reference you quote need to magically multiply their results by 1.7 to get good correlation and you only need 1.2 it shows that your model is better than theirs. But this magic is not good and you want to get accurate enough results without requiring magic numbers.

[keg504]

I don't like the magic number multiplication either, since it's not rigorously defined, it's the only way I can see to explain my results in the report right now.

At the tip, the Re number is ~300,000, and the whole blade seems to be in turbulent airflow. No stall as far as I can tell, but I may be wrong, as I'm not quite familiar with how to visualise stall (i.e. which variables to plot). The flow looks like it stays mostly attached, but I'm no expert, I'm trying to learn.

You can see the plots here:
Pressure on blade surface


Velocity near tip of blade:


Turbulent energy near tip: