# The problem of unsteady state calculation of propeller static thrust.

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

March 19, 2014, 00:01
The problem of unsteady state calculation of propeller static thrust.
#1
New Member

Xiaohua Li
Join Date: Nov 2013
Posts: 8
Rep Power: 3
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!
Attached Images
 export1.jpg (94.6 KB, 23 views) export2.jpg (68.4 KB, 22 views) problem2.jpg (90.8 KB, 21 views) problem4.JPG (69.0 KB, 18 views) problem5.JPG (51.0 KB, 11 views)

Last edited by liulangdefeng2222; March 20, 2014 at 00:09.

 March 19, 2014, 06:04 #2 Senior Member   Gonzalo Join Date: Mar 2011 Location: Argentina Posts: 108 Rep Power: 7 May be is the reference frame in which they are calculated. If so, you should use velocity in a stationary reference frame.

March 19, 2014, 06:17
#3
New Member

Xiaohua Li
Join Date: Nov 2013
Posts: 8
Rep Power: 3
Quote:
 Originally Posted by gfoam 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.

Last edited by liulangdefeng2222; March 19, 2014 at 23:58.

March 20, 2014, 00:07
#4
New Member

Xiaohua Li
Join Date: Nov 2013
Posts: 8
Rep Power: 3
Quote:
 Originally Posted by liulangdefeng2222 I use the Fluent 6.3.26 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!
can someone give me a favor?

March 20, 2014, 19:24
#5
Senior Member

Gonzalo
Join Date: Mar 2011
Location: Argentina
Posts: 108
Rep Power: 7
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
Quote:
 I want to calculate the static force, how to set velocity in a stationary reference frame?
, 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

March 21, 2014, 09:40
#6
New Member

Xiaohua Li
Join Date: Nov 2013
Posts: 8
Rep Power: 3
D300_SMM22353-1-0.jpg

D300_SMM22353-1-01100.jpg

Quote:
 Originally Posted by gfoam 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
Thank 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.

 March 21, 2014, 18:44 #7 Senior Member   Gonzalo Join Date: Mar 2011 Location: Argentina Posts: 108 Rep Power: 7 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

March 21, 2014, 20:36
#8
New Member

Xiaohua Li
Join Date: Nov 2013
Posts: 8
Rep Power: 3
Quote:
 Originally Posted by gfoam 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.

March 24, 2014, 20:08
#9
Senior Member

Gonzalo
Join Date: Mar 2011
Location: Argentina
Posts: 108
Rep Power: 7
Quote:
 I have simulate the situation from 3000r/min to 9000r/min, every time, the toroidal streamline appears, Whether it is normal?
: 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

March 24, 2014, 23:59
#10
New Member

Xiaohua Li
Join Date: Nov 2013
Posts: 8
Rep Power: 3
Quote:
 Originally Posted by gfoam : 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.

 March 25, 2014, 09:03 #11 Senior Member   Gonzalo Join Date: Mar 2011 Location: Argentina Posts: 108 Rep Power: 7 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

 July 7, 2015, 11:17 #12 New Member   Julia Join Date: May 2011 Posts: 12 Rep Power: 6 Hi I simulate a propeller in CFX. how can I calculate the thrust ?

 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 mahdisajjadi FLUENT 1 December 1, 2014 21:24 MASOUD Fluent UDF and Scheme Programming 0 June 5, 2010 00:49 Bogey Jammer Main CFD Forum 0 September 29, 2009 17:06 miguelin_us FLUENT 0 September 2, 2009 00:31 sm FLUENT 0 November 7, 2007 02:26

All times are GMT -4. The time now is 12:22.