# Lift forces generated by a Coanda UAV model

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 April 7, 2016, 03:17 Lift forces generated by a Coanda UAV model #1 New Member   Gordon Yeo Join Date: Jan 2016 Posts: 8 Rep Power: 3 Hi everyone, someone or anyone that can help me out here, I am currently doing a CFX simulation on a Coanda UAV model. I am generating lift value of the UAV by using the function calculator. See 'lift values coanda uav.jpg' lift values coanda uav.jpg The blue surface covers the coanda uav fuselage surface, which includes both the top and bottom surface of the uav. the fuselage is of bowl shape, so the underside of the uav is actually empty. As you can see, the lift forces calculated by the function calculator is of -0.9N which is different from my empirical lift data of approximately 10N. See 'velocity contour coanda uav.jpg' velocity contour coanda uav.jpg The velocity simulated seems to be pretty accurate when compared to empirical airflow velocity data taken by an anemometer at both the point circled in the picture attached. I believe my simulation is done in a wrong way as the rotating domain encircling the propeller is made to spin clockwise against the static anti-clockwise propeller to generate accelerate airflow down to the fuselage. My question: See 'iso view coanda uav.jpg' iso view coanda uav.jpg Is there another way that I should be using to calculate lift in this simulation? with regards to rotating domain against a static propeller, what is the correct way to approacj such simulation? I will deeply appreciate if anyone can help me with this! Thank you.

 April 7, 2016, 04:08 #2 Member   Aleksandr Join Date: Dec 2015 Location: Kharkov, Ukraine Posts: 74 Blog Entries: 1 Rep Power: 3 I think, first oa all, is bad mesh

 April 7, 2016, 04:14 #3 Senior Member   urosgrivc Join Date: Dec 2015 Location: Slovenija Posts: 199 Rep Power: 4 you could do a static analisis of the problem and as it is simetric you could simulate only one half of the problem (1/2 as propeler has 2 blades) And you must use inflation layers and finer mesh for this as it is seen from velocity that something is probably wrong with the mesh. with static analisis (frozen rotor) and symetry you coud make a lot finer mesh. If you just want lift datta this is a static analisis.

April 7, 2016, 04:17
#4
New Member

Gordon Yeo
Join Date: Jan 2016
Posts: 8
Rep Power: 3
Quote:
 Originally Posted by metaliat93 I think, first oa all, is bad mesh
Quote:
 Originally Posted by urosgrivc you could do a static analisis of the problem and as it is simetric you could simulate only one half of the problem (1/2 as propeler has 2 blades) And you must use inflation layers and finer mesh for this as it is seen from velocity that something is probably wrong with the mesh. with static analisis (frozen rotor) and symetry you coud make a lot finer mesh.
Hi, thanks for the prompt reply! I agree that it's a poor mesh as I will like to save on solving time while getting my set up right.

Would you think that a finer mesh with inflation alone on the fuselage surface will give me a lift value that will be accurate to my empirical results?

April 7, 2016, 04:23
#5
Member

Aleksandr
Join Date: Dec 2015
Location: Kharkov, Ukraine
Posts: 74
Blog Entries: 1
Rep Power: 3
Quote:
 Originally Posted by gordonhere Would you think that a finer mesh with inflation alone on the fuselage surface will give me a lift value that will be accurate to my empirical results?
unambiguously

 April 7, 2016, 04:38 #6 Senior Member   urosgrivc Join Date: Dec 2015 Location: Slovenija Posts: 199 Rep Power: 4 Yes mesh definitely And realy think about (static analisys) as i see you have velociti at t=5s what if the flow hasnt developed yet... It just takes to much computing power to solve a transient case like this plus you dont need it. And for the enclosure it would be beter if it would be a circular shape like ewerithing alse is.

 April 7, 2016, 05:00 #7 New Member   Gordon Yeo Join Date: Jan 2016 Posts: 8 Rep Power: 3 Okay! I'm on it. So you're implying that I should have these specified: Under 'Analysis type' Steady state analysis Under 'Interfaces' Frame change/Mixing Model: Frozen rotor Pitch change: None? (I have little clue about this) Edit: Also under my rotating domain enclosing the propeller Should my domain be rotating in the clockwise direction against my stationary anticlockwise-designed propeller blades or Should my domain be stationary while having an anticlockwise rotating wall specified under my blades boundary conditions In the mean time, I am working on a symmetric model to reduce the computing time and space required! Really thankful for your advice thus far :')

 April 7, 2016, 05:48 #8 Senior Member   urosgrivc Join Date: Dec 2015 Location: Slovenija Posts: 199 Rep Power: 4 You should get a good solution with frozen rotor (Steady state analysis) simulation. You must create two domains. Larger one will be stationary. Domain enclosing the propeler must be rotating - (wall motion wont work! as mesh would have to deform) Spin it in the direction as the propeler would be turning. (wals of the propeler are by default rotating with the domain) One Interface for frozen rotor should be set with pich change set to none. (if any problems ocure when solving -> make 2 interfaces - one for axial faces and one for radial cilinder connection) (not sure why but it worked for me in the past) Dont forget about the ciclic symetry rotational interface conection You will have to make 2 interfaces for ciclic periodicity One to connect both sides of rotating domain and one to conect both sides of stationary domain Refine the mesh on the surfaces and add inflation layers (personaly I would go for SST model and Y+<1 values on the propeler faces) (you can check y+ in CFXpost and than do a beter mesh if necesery. What is the speed of the tip of the propeler? -> if it is larger than (0,1-0,3 mach) use Air ideal gas Have fun

April 7, 2016, 22:00
#9
New Member

Gordon Yeo
Join Date: Jan 2016
Posts: 8
Rep Power: 3
Quote:
 Originally Posted by urosgrivc You should get a good solution with frozen rotor (Steady state analysis) simulation. You must create two domains. Larger one will be stationary. Domain enclosing the propeler must be rotating - (wall motion wont work! as mesh would have to deform) Spin it in the direction as the propeler would be turning. (wals of the propeler are by default rotating with the domain) One Interface for frozen rotor should be set with pich change set to none. (if any problems ocure when solving -> make 2 interfaces - one for axial faces and one for radial cilinder connection) (not sure why but it worked for me in the past) Dont forget about the ciclic symetry rotational interface conection You will have to make 2 interfaces for ciclic periodicity One to connect both sides of rotating domain and one to conect both sides of stationary domain Refine the mesh on the surfaces and add inflation layers (personaly I would go for SST model and Y+<1 values on the propeler faces) (you can check y+ in CFXpost and than do a beter mesh if necesery. What is the speed of the tip of the propeler? -> if it is larger than (0,1-0,3 mach) use Air ideal gas Have fun
Tip speed is 99m/s - 0.29 mach. I am now using ideal gas air.

However, I encountered this problem:

Quote:
 Originally Posted by gordonhere +--------------------------------------------------------------------+ | Host Memory Information (Mbytes) | +--------------------------------------------------------------------+ | Host | Npart | System | Allocated | % | +------------------------+-------+-------------+-------------+-------+ | GORDON | 4 | 7813.53 | 10340.84 |132.35 | +------------------------+-------+-------------+-------------+-------+ +--------------------------------------------------------------------+ | ERROR #333100220 has occurred in subroutine Out_MemPar. | | Message: | | | | The allocated memory exceeds the system memory on 1 host(s). | | | | The logical expert parameter "enforce system memory limit" | | controls whether this is a fatal error. | | | | The current setting is: fatal | | | | Allocating more than the system memory may result in slow or | | unreliable operation and is not recommended. | +--------------------------------------------------------------------+ +--------------------------------------------------------------------+ | An error has occurred in cfx5solve: | | | | The ANSYS CFX solver exited with return code 1. No results file | | has been created. | +--------------------------------------------------------------------+ End of solution stage. +--------------------------------------------------------------------+ | The following user files have been saved in the directory D:/Final | | Year Project/Simulations/Symmetrical simulation/Symmetrical | | simulation_pending/dp0_CFX_Solution/CFX_001: | | | | pids | +--------------------------------------------------------------------+ +--------------------------------------------------------------------+ | For CFX runs launched from Workbench, the final locations of | | directories and files generated may differ from those shown. | +--------------------------------------------------------------------+ +--------------------------------------------------------------------+ | Warning! | | | | After waiting for 60 seconds, 1 solver manager process(es) appear | | not to have noticed that this run has ended. You may get errors | | removing some files if they are still open in the solver manager. | +--------------------------------------------------------------------+ This run of the ANSYS CFX Solver has finished.
This simply means that my computer do not have enough computing power right?

 April 7, 2016, 23:14 #10 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,068 Rep Power: 109 You clearly need to do sensitivity analyses on mesh and converge tolerance. I recommend that you this by: * a 2D axisymmetric model for the main body, using a momentum source term for the low from the rotor * a 3D rotating frame of reference simulation for the rotor As these models are much simpler and smaller than your full model you should not have memory problems. Once you have determined the mesh required for the body and rotor in these simpler models then you can combine them together with some hope that the full model will be accurate.

 April 8, 2016, 01:24 #11 Senior Member   urosgrivc Join Date: Dec 2015 Location: Slovenija Posts: 199 Rep Power: 4 Mr. Glenn gave good suggestions 2D simulation would be very fast indeed (But you would have to specify inlet BC, without using the propeler) Yes the erorr (in general) means that the mesh has to much nodes. If you still want tu run the soulution reduce the mesh number of nodes for at least 35% or more. Solution will than be able to run but sesitivity check must be done. Do not believe your first results as these still might be wrong due to (lots of factors you didnt include or check->(is the enclosure big enough, is the inflation fine enough, is the model wright for the job...?) Solution (lift force) must be independant of those factors - that is sensitivity check. Personaly I think you just might be able to do it with only 8Gb of ram (with simetry) As the mesh can have more than Milion nodes still. I gues you have about 2M now (I realy want to know (to check how far I was)) Later i was thinking that you wouldnt even need two domains for this problem, one rotating one shoul be enough. And think about slicing the enclosure in to more pieces as you could generate structured mesh asweal, that would save some precious nodes (becouse of small ram size) so you could put elements where you really need them

April 10, 2016, 11:32
#12
New Member

Gordon Yeo
Join Date: Jan 2016
Posts: 8
Rep Power: 3
Quote:
 Originally Posted by ghorrocks You clearly need to do sensitivity analyses on mesh and converge tolerance. I recommend that you this by: * a 2D axisymmetric model for the main body, using a momentum source term for the low from the rotor * a 3D rotating frame of reference simulation for the rotor As these models are much simpler and smaller than your full model you should not have memory problems. Once you have determined the mesh required for the body and rotor in these simpler models then you can combine them together with some hope that the full model will be accurate.
Quote:
 Originally Posted by urosgrivc Mr. Glenn gave good suggestions 2D simulation would be very fast indeed (But you would have to specify inlet BC, without using the propeler) Yes the erorr (in general) means that the mesh has to much nodes. If you still want tu run the soulution reduce the mesh number of nodes for at least 35% or more. Solution will than be able to run but sesitivity check must be done. Do not believe your first results as these still might be wrong due to (lots of factors you didnt include or check->(is the enclosure big enough, is the inflation fine enough, is the model wright for the job...?) Solution (lift force) must be independant of those factors - that is sensitivity check. Personaly I think you just might be able to do it with only 8Gb of ram (with simetry) As the mesh can have more than Milion nodes still. I gues you have about 2M now (I realy want to know (to check how far I was)) Later i was thinking that you wouldnt even need two domains for this problem, one rotating one shoul be enough. And think about slicing the enclosure in to more pieces as you could generate structured mesh asweal, that would save some precious nodes (becouse of small ram size) so you could put elements where you really need them
Hi there, I've been experimenting the mesh and also putting this 2d model together. But I'm not sure if it's exactly what Mr Glenn meant. I've attached screenshots here. Could you clarify if this is what was meant? thanks! and it is 1cm thick.

2d geog.jpg 2d geog - rotating domain closeup.jpg
but what do you mean by momentum source term for low from the rotor?

And yes! I was around 2M

 April 10, 2016, 18:33 #13 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,068 Rep Power: 109 Rather than use a momentum source it would be simpler to use an inlet boundary as suggested by urosgrivc. Also, your model is 2D axisymmetric, not planar 2D so you should do a 2D axisymmetric model.

April 11, 2016, 02:17
#14
New Member

Gordon Yeo
Join Date: Jan 2016
Posts: 8
Rep Power: 3
Quote:
 Originally Posted by ghorrocks Rather than use a momentum source it would be simpler to use an inlet boundary as suggested by urosgrivc. Also, your model is 2D axisymmetric, not planar 2D so you should do a 2D axisymmetric model.
Okay, so I'll remove the propeller and have an simple circular inlet instead. Sorry, I misunderstood when you mention 2D!

Anyway, I've done out a axis-symmetric model this time, i hope i got it right this time! converged on the 63rd iterations with a RMS residual target of 1e-04. But the results is quite different from my 3d geog simulation. I'm guessing that my inlet geog or inlet velocity isn't the set in the best way to give me identical result when compared to my 3d geog.

Here's a 2 screenshots of the velocity contour in 2d and 3d simulation
3d full geog velocity contour.jpg axissymetric velocity contour.jpg

Also, the lift force generated over my fuselage is of negative magnitude. Am I measuring lift wrongly..? This is just a quadrant of the model, is there anyway where I can duplicate the other 3 quadrants to complete a full model in CFD-Post?
axissymmetric lift force.jpg

Really really appreciate the help and accommodating to my question thus far!

 April 11, 2016, 02:38 #15 New Member   Gordon Yeo Join Date: Jan 2016 Posts: 8 Rep Power: 3 i think this might be helpful for the help i can receive! openings axissymmetric.jpg inlet axissymmetric.jpg these shows the boundary conditions that i had set for the 'inlet disk' that hangs in the mid air of the default domain

 April 12, 2016, 01:03 #16 Senior Member   urosgrivc Join Date: Dec 2015 Location: Slovenija Posts: 199 Rep Power: 4 To check convergence; You must make a monitor point Force_y@(location) this will show you lift. With this you are able to see lift value while the solver solves the problem, and when it stops changing the convergence is reched. RMS residual target of 1e-04 is in meny cases not good. I never rely only on RMS residuals. Last edited by urosgrivc; April 12, 2016 at 02:09.

 April 12, 2016, 06:09 #17 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,068 Rep Power: 109 Also you missed the point of the axisymmetric suggestion. Your mesh has a 90 degree slice with many elements through the thickness. I was intending it to be a thin slice - maybe 2 or 3 degrees, and only 1 element thick. This means you are using the minimum elements in the thickness direction and can put all the refinement in resolving the object's boundary layer. urosgrivc likes this.

April 15, 2016, 11:59
#18
New Member

Gordon Yeo
Join Date: Jan 2016
Posts: 8
Rep Power: 3
Quote:
 Originally Posted by urosgrivc To check convergence; You must make a monitor point Force_y@(location) this will show you lift. With this you are able to see lift value while the solver solves the problem, and when it stops changing the convergence is reched. RMS residual target of 1e-04 is in meny cases not good. I never rely only on RMS residuals.
Quote:
 Originally Posted by ghorrocks Also you missed the point of the axisymmetric suggestion. Your mesh has a 90 degree slice with many elements through the thickness. I was intending it to be a thin slice - maybe 2 or 3 degrees, and only 1 element thick. This means you are using the minimum elements in the thickness direction and can put all the refinement in resolving the object's boundary layer.
Hi guys, sorry for the radio silence! but i will really to thank the both of you for the thus far! This is what i've managed

velocitycontour.jpg yplus.png

The results are satisfactory i tried to use an normal inlet bc to replace the propeller, however the flow is of constant velocity in the radial direction of the inlet disk which is not true when compared to a propeller

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Maddy FLUENT 9 September 10, 2017 05:27 musabai OpenFOAM Running, Solving & CFD 2 February 20, 2015 15:07 vikhattangady FLUENT 0 October 31, 2013 05:42 wake ANSYS Meshing & Geometry 0 December 4, 2009 05:15 Victor Serov Main CFD Forum 19 August 15, 1999 23:45

All times are GMT -4. The time now is 19:44.

 Contact Us - CFD Online - Privacy Statement - Top