# Wind Turbine DFBI

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

 April 15, 2013, 21:51 Wind Turbine DFBI #1 New Member   BKaiser Join Date: Sep 2012 Posts: 4 Rep Power: 7 Hello, I am attempting to model a rotating wind turbine using the dynamic fluid body interaction (DFBI) solver in STAR CCM+. I've constrained the turbine (floating in the center of the control volume, no tower) to rotate about the axis it would in reality, set an initial rotational velocity, moments of inertia, ramp time, release time, etc. I have one region, with many surfaces, and DFBI turned on. My DFBI body is the turbine, which is also it's own surface within the region. For some reason, the turbine surface still expects a specified rotation rate, even though I already specified an initial one in my DFBI body. Near the end of ramp time, the rotation was faster than the specified initial rotation, and the solver seemed to disregard the specified rotation rate for the surface. Did I do the simulation correctly, and if so, why does it ask for a specified rotation rate for the surface which it seems to not use? Also, I had pictures out put from each time step and STAR appears to be rotating my entire mesh, not just the turbine. STAR crashes when I try to see the geometry, scalar, or mesh scenes. Thanks in advance! I apologize for the long question.

 April 16, 2013, 10:20 #2 Member   Ryan Coe Join Date: Jun 2010 Location: Albuquerque, NM Posts: 98 Rep Power: 9 How are you achieving the rotation of the turbine blades? Are the blades located within their own cylindrical embedded region? __________________ Ryan

 April 17, 2013, 20:46 #3 New Member   BKaiser Join Date: Sep 2012 Posts: 4 Rep Power: 7 Hi Ryan, No, I just set the initial rotation for that part only, assuming that the way STAR works in this case is to treat the rotation like a boundary condition...but it seems like that is not correct. Do I need to embed the turbine in a separate mesh? Thanks! -Bryan

 April 17, 2013, 21:21 #4 Member   Ryan Coe Join Date: Jun 2010 Location: Albuquerque, NM Posts: 98 Rep Power: 9 From what I can tell from your description of the simulation you want to run, yes you do need to have a separate region for the turbine blade. This allows the blade to rotate and the rest of the domain to remain inertially fixed. __________________ Ryan

 April 19, 2013, 14:19 #5 New Member   BKaiser Join Date: Sep 2012 Posts: 4 Rep Power: 7 Thanks Ryan! I will go back to the demos for that then. I've been looking at the moving reference frame approach, and STAR says it's "not suitable for resolving flow structures, e.g. wake coming off rotating machinery"... do you recommend another method in STAR for wakes coming off rotating machinery?

 April 19, 2013, 15:20 #6 Senior Member   Join Date: Mar 2009 Location: Austin, TX Posts: 147 Rep Power: 11 You need to use sliding mesh. Also, you need to start with a simpler simulation. Do not start with the monster DFBI simulation. Start with a steady-state rotating reference frame simulation, then use that result as the initial conditions for a transient sliding mesh simulation and experiment to find a suitable mesh size and time step. Only then should you even be thinking about enabling DFBI.

 April 19, 2013, 15:38 #7 New Member   BKaiser Join Date: Sep 2012 Posts: 4 Rep Power: 7 Hi Kyle, Thanks, yes I just went over the MRF demo, and will run some basic simulations before progressing up to DFBI. Do you know what degree of accuracy STAR's RANS models are capable of for predicting wake flow structure? I'm wondering if there is information regarding what I can expect when I get there. Thanks, -Bryan

 April 19, 2013, 15:49 #8 Senior Member   Join Date: Mar 2009 Location: Austin, TX Posts: 147 Rep Power: 11 It really depends on your geometry and your goals. If you are simulating a turbine with 2 or 3 blades, then no steady-state simulation is going to even come close to resolving the wake accurately. If your geometry is a windmill with 50+ blades then a simple steady-state RANS MRF simulation might actually do a reasonably good job. This has nothing to do with STAR's capabilities, it just can't calculate things that you don't ask it to calculate. Moving reference frame simulations will always be less accurate than sliding mesh because MRF can only calculate for a single physical position of the moving geometry. Sometimes it's close enough, sometimes it isn't. Last edited by kyle; April 19, 2013 at 17:21.

 August 1, 2013, 20:47 #9 New Member   malu Join Date: Jun 2013 Posts: 8 Rep Power: 6 is there any limitation using the rotating mesh and eulerian multiphase models simultaneously?? I'm modelling a rotating blade over which gas-liquid mixture flows. Once i turn on the rotation, the AMG solver diverges. Thanks.

 Tags boundaries condition, dfbi, fsi, rotation, star ccm+

 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 Pepita CFX 4 June 29, 2013 07:09 kongl1986 FLUENT 0 March 30, 2013 11:50 atorninc Main CFD Forum 3 March 6, 2013 05:38 AUN CFX 13 August 29, 2012 16:44 Saturn FLUENT 1 June 16, 2006 02:12

All times are GMT -4. The time now is 01:56.