The problem of unsteady state calculation of propeller static thrust.
 

I use the Fluent 14 to calculate the propeller static thrust in unsteady state.
boundary conditon: inlet: pressure inlet; outlet: pressure outlet; flowfied cylinder: preussure inlet; Using interface to connect the ratary region and stationary region.
tuanblence model: k-e(RNG)
Using moving mesh, the ratation speed is 9000r/min
the result of the force and moment is consistent with the experimental results. BUt the streamline is strange.
Dose anyone have good idear? could you give me a favor? thank you very much!

May be is the reference frame in which they are calculated. If so, you should use velocity in a stationary reference frame.

I am sorry,I don't understand your meaning. I want to calculate the static force, how to set velocity in a stationary reference frame? Could you please explain in detail?
thank you very much.

can someone give me a favor?

Sorry for the late response, I've been a little bussy in thees days. But I don't understand you very well, you want to calculate the static force or the streamlines? Because you said that your results of static force are in agreement with the experimental data an then you said , never mind. If you want to calculate the streamlines when you have a sliding mesh you mus use the velocities referenced to a inertial reference frame. Please take a look at this link. But it says that the velocities utiliced in fluen for postprocessing are referenced in a stationary frame by default. So, the problem may be other. Could you give me some details like timestep, number of time steps used, mesh size, solver used, discretization, and so on. The problem may arise from many places!
And if you have acces to CFDPost try to plot the streamlines in there and show me what you get. Regards.
Gonzalo

Attachment 29528

Attachment 29529

Attachment 29530Thank you very much for your reply. I have use CFDPost and tecplot to plot the streamline. You can have a look. I want use Fluent to calculate the force and moment at the speed of 9000r/min. The result of force and moment is good. But when I use CFDPost see the Velocity contours and pathline, I think it dosen't not consistent with physical reality and not find the reason. I use sovler of pressure-based, k-e model(RNG), time step(0.0001s),number of time steps:10000.
If you have a good idear, You can also send me an email: lixh0208@sina.com appreciate.

One more question, the external velocity of the fluid is zero? If so, the phenomena you are facing could be possible. I mean, if the propeler has a high load, it could absorb fluid from all the surrounding space even the one is behind the plane of the propeller but not under the disk plane. Do I make myself clear? Is rather difficult to explain. This occurs in the case of engines at full power and zero velocity. Then such pattern of streamlines could appear. Let me know if the velocity of the free stream is non zero, and we can find another solution.
But that explains the toroidal streamlines near the plane of the propeller, the other streamlines could apperar for the same reason (zero frestream velocity) but generated by an exchange in momentun by shear forces between the slipstream of the propeller and the stationary fluid, I don't know, it could be possible???? Let me know if we could do something else. Regards
Gonzalo

Yes，the external velocity of the fluid is zero and the velocity of the free streamline is zero. I can understand the fluid surrrouding propller is absorbed. But I can't explain the toroidal streamline near the plane of propeller, you said the exchange in momentun by shear forces between the slipstream of the propeller and the stationary fluid makes sense.
I have simulate the situation from 3000r/min to 9000r/min, every time, the toroidal streamline appears, Whether it is normal?
Thank you so much.

: Following my line of thoughts I think yes, no matter the angular velocity you put to the propeller you will have that kind of toroidal streamlines provided that you have traction, because you always have velocity behind the propeller's slipstream and exchange of momentum. I recommend you, if you can afford it (time specially) simulate the same propeller with the same angular velocity but with non zero free stream velocity and see what happens.
One more time, because you never answer me: are you sure thet you used "Velocity in Stn Frame" in CFDPost to plot the streamlines?
I hope this helps you, regards. Gonzalo

At first, I want to tell a good news that I have find the problem. The problem is just the calculation of the intermediate state， it hasn't reached steady state. After nearly four days calculation time, I found that the toroidal streamlines disappeared, and the streamline is nearly similar as the calculation result by using MRF model.
I have also simulate the situation that the stream velocity is 20m/s, it just uses several hous to get steady, and has no toroidal streamlines .
I am so that I didn't explain clearly, I don't use "Velocity in Stn Frame".
Thank you so much for helping me.

I'm glad you found you problem, may be that was the first thing that I had to ask you: did your simulation reach a steady state? Hehe, but well you found your problem and solved it. It seems that in the transition to a stady state the toroidal streamlinees apperar and then disappear when the fluid surrounding the slipstream has certain velocity induced by the former, mmm could be possible. Well, CU in another post. Regards.
Gonzalo

Hi

I simulate a propeller in CFX. how can I calculate the thrust ?