CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Propeller simulation not matching experimental data

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree12Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 18, 2024, 09:05
Default New simulation results
  #21
Member
 
Kevin Gnanaraj
Join Date: Apr 2024
Posts: 34
Rep Power: 2
keg504 is on a distinguished road
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:
keg504 is offline   Reply With Quote

Old   April 18, 2024, 09:52
Default
  #22
Senior Member
 
Join Date: Jun 2009
Posts: 1,875
Rep Power: 33
Opaque will become famous soon enough
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.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   April 18, 2024, 10:19
Default Timescale
  #23
Member
 
Kevin Gnanaraj
Join Date: Apr 2024
Posts: 34
Rep Power: 2
keg504 is on a distinguished road
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?
keg504 is offline   Reply With Quote

Old   April 18, 2024, 11:21
Default
  #24
Senior Member
 
Join Date: Jun 2009
Posts: 1,875
Rep Power: 33
Opaque will become famous soon enough
Quote:
Originally Posted by keg504 View Post
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.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   April 18, 2024, 20:33
Default
  #25
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,862
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   April 19, 2024, 13:42
Default Results with new timesteps
  #26
Member
 
Kevin Gnanaraj
Join Date: Apr 2024
Posts: 34
Rep Power: 2
keg504 is on a distinguished road
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:




Opaque likes this.
keg504 is offline   Reply With Quote

Old   April 19, 2024, 23:36
Default
  #27
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,862
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   April 22, 2024, 07:12
Default Boundary jet
  #28
Member
 
Kevin Gnanaraj
Join Date: Apr 2024
Posts: 34
Rep Power: 2
keg504 is on a distinguished road
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:
keg504 is offline   Reply With Quote

Old   April 22, 2024, 07:38
Default
  #29
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,862
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   April 22, 2024, 10:21
Smile Results of splitting opening
  #30
Member
 
Kevin Gnanaraj
Join Date: Apr 2024
Posts: 34
Rep Power: 2
keg504 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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 likes this.
keg504 is offline   Reply With Quote

Old   April 22, 2024, 13:20
Default
  #31
Senior Member
 
Join Date: Jun 2009
Posts: 1,875
Rep Power: 33
Opaque will become famous soon enough
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.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   April 22, 2024, 19:13
Default
  #32
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,862
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
Opaque and keg504 like this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   April 29, 2024, 17:39
Default Grid study
  #33
Member
 
Kevin Gnanaraj
Join Date: Apr 2024
Posts: 34
Rep Power: 2
keg504 is on a distinguished road
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

Last edited by keg504; April 29, 2024 at 18:04. Reason: fixed incomprehensible sentence, added a possible epiphany
keg504 is offline   Reply With Quote

Old   April 29, 2024, 18:47
Default
  #34
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,862
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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 likes this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   May 1, 2024, 09:48
Default New result
  #35
Member
 
Kevin Gnanaraj
Join Date: Apr 2024
Posts: 34
Rep Power: 2
keg504 is on a distinguished road
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
keg504 is offline   Reply With Quote

Old   May 1, 2024, 14:13
Default
  #36
Senior Member
 
Join Date: Jun 2009
Posts: 1,875
Rep Power: 33
Opaque will become famous soon enough
Quote:
Originally Posted by keg504 View Post
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.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   May 1, 2024, 15:30
Default
  #37
Member
 
Kevin Gnanaraj
Join Date: Apr 2024
Posts: 34
Rep Power: 2
keg504 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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 is offline   Reply With Quote

Old   May 5, 2024, 11:50
Default RPM variation
  #38
Member
 
Kevin Gnanaraj
Join Date: Apr 2024
Posts: 34
Rep Power: 2
keg504 is on a distinguished road
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
keg504 is offline   Reply With Quote

Old   May 5, 2024, 19:27
Default
  #39
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,862
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   May 6, 2024, 08:02
Default
  #40
Member
 
Kevin Gnanaraj
Join Date: Apr 2024
Posts: 34
Rep Power: 2
keg504 is on a distinguished road
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:
keg504 is offline   Reply With Quote

Reply

Tags
floating point exception, mixing planes, propeller flow error

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[OpenFOAM] Paraview python script, creating data using only CLI, saving in csv/excel file Ash Kot ParaView 1 September 24, 2021 13:23
Error running AMI propeller simulation luitzor OpenFOAM Running, Solving & CFD 0 April 19, 2021 14:48
Pump CAD + experimental data for CFD verification study bemism Main CFD Forum 0 July 20, 2017 16:30
Data Produced From Fine Marine Cant Match with The Experimental Data PeiSan Fidelity CFD 4 August 23, 2014 06:33
How to compare the average velocity of the simulation with the Experimental data ? nanavati OpenFOAM Post-Processing 2 August 22, 2014 05:48


All times are GMT -4. The time now is 09:38.