CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Quadrotor helicopter propeller simulation (http://www.cfd-online.com/Forums/cfx/71591-quadrotor-helicopter-propeller-simulation.html)

Attesz January 8, 2010 12:38

Quadrotor helicopter propeller simulation
 
5 Attachment(s)
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.

http://www.cfd-online.com/Forums/att...1&d=1262968530

Attachment 1938
Attachment 1937
Attachment 1936
If you need more information, let me know!

Thanks for any advice!

Regards,
Attesz

Abou ali January 8, 2010 14:36

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?????!!!!

sans January 9, 2010 02:14

Quote:

Originally Posted by Attesz (Post 241905)
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.

Attesz January 9, 2010 09:43

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

Attesz January 9, 2010 16:23

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

sans January 11, 2010 00:29

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.

Attesz January 11, 2010 07:31

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

ghorrocks January 11, 2010 17:56

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.

Attesz January 11, 2010 18:02

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

ckleanth January 11, 2010 20:45

http://www.cfd-online.com/Forums/cfx...html#post66243

read post 7

Attesz January 12, 2010 04:06

Thank you ckleanth!

ghorrocks January 12, 2010 18:00

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)

D.B August 31, 2012 04:06

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.


All times are GMT -4. The time now is 12:56.