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

Quadrotor helicopter propeller simulation

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

Like Tree2Likes
  • 1 Post By Attesz

Reply
 
LinkBack Thread Tools Display Modes
Old   January 8, 2010, 12:38
Lightbulb Quadrotor helicopter propeller simulation
  #1
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
Hi,

I'm simulating a quad rotor helicopter's propeller (only one). During my work, the simulation reaches the convergence very strange, I think. The RMS residuals, domain imbalances are converged, but the monitor points: force on the propellers and the mass flow seems to be not. How can it be, that the imbalances are under 0.0001 but the mass flow "curve" is not constant?

Information:

I'm using ICEM to generate mesh. Cell number: about 800.000. In boundary layer I'm using 5 cells, and the yplus value are under 2, at most under 1. The mesh is fine around the blades and the leading and trailing edges, and of course between the blade tip and wall.

Simulation properties: Steady run, SST turbulence model, 5000 RPM rotational velocity, Frozen Rotor interface type, inlet: total pressure with zero gradient turb, outlet stat pressure with medium intensity, each pressures are 1 bar (0 relative). Timescale: Automatic with Agressive lenght scale option. Initialization: velocity and pressure, with estimated values.

My problem is, that why cannot reach the simulation convergence under 1000 step, and how can I speed up the simulation? It seems to be, that that the massflow and forces can't converge, but RMS values are good.



RMS.jpg
massflow.jpg
force.jpg
If you need more information, let me know!

Thanks for any advice!

Regards,
Attesz
Attached Images
File Type: jpg assembly.jpg (27.3 KB, 541 views)
File Type: jpg assembly2.jpg (20.6 KB, 135 views)
mr.dargahi likes this.
Attesz is offline   Reply With Quote

Old   January 8, 2010, 14:36
Default
  #2
Member
 
Join Date: Nov 2009
Posts: 49
Rep Power: 7
Abou ali is on a distinguished road
Hi,
I have some observations about your work, maybe it can help,
1- You used 5 cells in the boundary layer but in the CFX help it is mentioned that a boundary layer should be resolved with at least of 15 nods for Low-R model.
2- To speed up your simulation convergence a high quality of mesh is required.
3- The stabilization of force and mass flow is not only function of RMS but also of MAX residual.
4- I see that error on those quantities is below 1% after 400 iterations, is this a problem?????!!!!
Abou ali is offline   Reply With Quote

Old   January 9, 2010, 02:14
Default
  #3
Member
 
SanS
Join Date: Mar 2009
Posts: 42
Rep Power: 8
sans is on a distinguished road
Quote:
Originally Posted by Attesz View Post
how can I speed up the simulation?
What is the time step your using? You may slowly ramp it up, this should speed up your convergence else it may even start to diverge. Read the Solver Help files for more information.
sans is offline   Reply With Quote

Old   January 9, 2010, 09:43
Default
  #4
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
Hi Abou ali, thank you for your answer!

Quote:
1- You used 5 cells in the boundary layer but in the CFX help it is mentioned that a boundary layer should be resolved with at least of 15 nods for Low-R model.
Ok, I will try it!

Quote:
2- To speed up your simulation convergence a high quality of mesh is required.
The mesh is good quality. To get better quality, I need to refine the mesh, which causes more time need.

Quote:
4- I see that error on those quantities is below 1% after 400 iterations, is this a problem?????!!!!
No, 1% is good enough, but You see, that after 1000 iterations, the values are increasing. It isn't problem? What if they continue to increase further during the iterations and thrust grows up? By comparing with the measures, we get bigger thrust values than in simulation...Therefore, I'm uncertain...


And one more question: what is the best way to measure thrust in simulation? So far, a plane was used, and the axial force acting on this figured out. Is it better, to calculate an average speed, and using the equation: m*c+A*(p-p0)?

Thank you once again,
Attesz

Last edited by Attesz; January 9, 2010 at 16:25.
Attesz is offline   Reply With Quote

Old   January 9, 2010, 16:23
Default
  #5
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
Quote:
What is the time step your using? You may slowly ramp it up, this should speed up your convergence else it may even start to diverge. Read the Solver Help files for more information.
I'm using steady simulation. The timescale is 2.38733E-04, which is automatically adjusted during run. I've set the Agressive Timescale option, which means a much bigger timescales. Do you recommend to set the timescale manually, bigger as the automatically setted one?

Thank you,
Attesz
Attesz is offline   Reply With Quote

Old   January 11, 2010, 00:29
Default
  #6
Member
 
SanS
Join Date: Mar 2009
Posts: 42
Rep Power: 8
sans is on a distinguished road
With an autotimescale you can take for ever to reach convergence. Ramp it by factor of 10 and then monitor your residuals and variables of interest. You could ramp it up as high as you can get away with.
sans is offline   Reply With Quote

Old   January 11, 2010, 07:31
Default
  #7
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
Hi sans,

I've started a simulation with Timescale Factor 10, it seems to be good. But this timescale wouldn't cause inaccuracy in results? After finish, should I run a few iterations with conservative timescale and Factor 1?

Thank you,
Attesz
Attesz is offline   Reply With Quote

Old   January 11, 2010, 17:56
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Are you sure your simulation has converged? It looks like you only have loose convergence to me and you could easily converge tighter. That may help things.
ghorrocks is offline   Reply With Quote

Old   January 11, 2010, 18:02
Default
  #9
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
Thanks Glenn, but ramping up with Timescale Factor, the RMS residuals have started to decrease rapidly, and also the mass&force values have stabilized, so sans's advice is working!

Attesz
Attesz is offline   Reply With Quote

Old   January 11, 2010, 20:45
Default
  #10
Senior Member
 
ckleanth's Avatar
 
George
Join Date: Mar 2009
Location: Birmingham, UK
Posts: 257
Rep Power: 9
ckleanth is on a distinguished road
convergence problem

read post 7
__________________
Top 4 tips
1. Knowledge is everything and Ignorance is dangerous.
2. Understand your limitations and try to eliminate them.
3. Get yerself a bike and hoon the chuffer. You will soon learn why dogs like to hang their heads out the car window.
4. Please before asking any questions on how to run simulations in CFX, go though all the tutorials
ckleanth is offline   Reply With Quote

Old   January 12, 2010, 04:06
Default
  #11
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
Thank you ckleanth!
Attesz is offline   Reply With Quote

Old   January 12, 2010, 18:00
Default
  #12
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Regardless, have you checked that your convergence is tight enough? You need to do a sensitivity check on it. (Run a tighter and looser convergence tolerance and see if the differences are significant for you)
ghorrocks is offline   Reply With Quote

Old   August 31, 2012, 04:06
Default
  #13
D.B
Member
 
DB
Join Date: Apr 2011
Posts: 62
Rep Power: 6
D.B is on a distinguished road
Hi,
I hope you have tried Delunay method of volume meshing in ICEM, if not I think you should cause it has HUGE effect on convergence as i have seen in some of my rotating machinery cases.
Also I agree with ghorrocks, your simulation seems a relatively simple one so you should have a tighter convergence criteria like RMS/MAX= 10-6, dont concentrate so much on imbalance, your monitors should be your primary criteria.
__________________
-D.B
D.B is offline   Reply With Quote

Reply

Tags
convergence, propeller, quadrotor

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Aircraft propeller simulation white FLUENT 2 January 13, 2014 05:20
Propeller Simulation Craig Paxton FLUENT 11 February 17, 2010 00:57
Propeller flow simulation jun005 Main CFD Forum 0 August 5, 2009 02:10
simulation of water flow though a ducted propeller spacewatcer FLUENT 0 April 22, 2009 09:52
Propeller Fan Curve Simulation Teng_YJ FLUENT 2 February 16, 2009 20:37


All times are GMT -4. The time now is 20:23.