# Rotating cylinder

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

 LinkBack Thread Tools Display Modes
 January 27, 2010, 13:47 Rotating cylinder #1 New Member   Join Date: Jan 2010 Posts: 4 Rep Power: 9 Hi everyone, I just started to use OpenFOAM and am currently studying the "Flow around a cylinder" tutorial. Suppose I want to see the effect of having the cylinder rotate. This would easily be configured by setting the boundary to moving wall and specifying the angular velocity. Is this possible? I have read about mesh motion mechanisms, but they seem like overkill in this case, since the mesh is not moving, only the cylinder wall is. Any help appreciated. Thanks, Ole

 January 27, 2010, 16:44 #2 Member   Patricio Bohorquez Join Date: Mar 2009 Location: Jaén, Spain Posts: 95 Rep Power: 10 That is an interesting problem. Could you use GGI boundary condition on the "inside" cylinder and keep us posted? You could try something similar to mixerGgi that lives into OpenFOAM-1.5-dev/tutorials/icoDyMFoam. Thanks, Patricio.

 January 27, 2010, 17:19 Using GGI changes problem to an unsteady one #3 New Member   Join Date: Jan 2010 Posts: 4 Rep Power: 9 Using GGI changes (as far as I understand) the problem to an unsteady one. I am interested in the steady solution, just like in the tutorial for the cylinder flow, except the cylinder should rotate with a constant speed. This amounts to setting the tangential velocity of the cylinder boundary to some uniform value, and then solving the steady problem. I can set the velocity on the boundary uniformly to some constant vector in cartesian coordinates, but is it possible to set the tangential velocity to some constant?

January 28, 2010, 11:32
#4
Senior Member

Andrea Pasquali
Join Date: Sep 2009
Location: Germany
Posts: 142
Rep Power: 10
You can try with this BC in U file

Quote:
 cilindro { type rotatingWallVelocity; origin (0 0 0); axis (0 0 1); omega 50; }
__________________
Andrea Pasquali

 January 28, 2010, 12:54 #5 New Member   Join Date: Jan 2010 Posts: 4 Rep Power: 9 Works perfectly! Thank you.

 February 2, 2010, 10:54 rotatingWallVelocity or MRFsimpleFoam #6 Senior Member     maddalena Join Date: Mar 2009 Posts: 436 Rep Power: 15 Hello everybody, I am wondering if a simpleFoam with a rotatingWallVelocity BC simulation can replace a MRFsimpleFoam simulation. They both are steadyState but: simpleFoam + rotatingWallVelocity: update the velocity considering the rotation, thus modify ALL the velocity term in the NS equations; MRFsimpleFoam: add a source term to the NS equations (see here). Anyone has studied the influence on results of these approach? Thanks to those that will shed some light! mad

 February 10, 2010, 05:45 Solved! #7 Senior Member     maddalena Join Date: Mar 2009 Posts: 436 Rep Power: 15 Ok, I find the answer with the help of a young woman far more expert in cfd modeling than me. The rotatingWall BC applies the rotation only the flow that is in contact with the wall, since it is a boundary condition. This will propagate to the adjacent cells but the rotating effect will be under-predicted since these cells have their own velocity that has no rotation component. This can be ok if the wall is simple, i.e. there are no blades on the rotating body. This is ok for the rotating cylinder case of this thread. On the other hand, the MFR approach considers as rotating the whole flow volume around the wall. This case is more adequate if the rotating body has blades. Indeed, the flow between two blades has almost the same velocity of the blades themselves. The MRF approach is ok if the mean flow far from the rotating body is wanted, or if the blade number is high, since the steady field values can be obtained only. If the blade number is low, the pressure pulse generated by the blade rotation cannot be discarded and a dynamicMesh approach should be used. Hope to be useful to someone else. Cheers, maddalena Soheyl, kiddmax, blake and 3 others like this.

 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 raul FLUENT 3 February 1, 2015 06:48 lbeaudet OpenFOAM Running, Solving & CFD 4 July 6, 2009 02:13 Tim Daly FLUENT 1 November 10, 2008 00:02 Jason Mc Beth FLUENT 0 January 23, 2008 08:02 Nick Siemens 1 June 21, 2006 06:42

All times are GMT -4. The time now is 05:14.

 Contact Us - CFD Online - Privacy Statement - Top