CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   STAR-CCM+ (http://www.cfd-online.com/Forums/star-ccm/)
-   -   Wind Turbine DFBI (http://www.cfd-online.com/Forums/star-ccm/116244-wind-turbine-dfbi.html)

BKaiser April 15, 2013 21:51

Wind Turbine DFBI
 
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.

ryancoe April 16, 2013 10:20

How are you achieving the rotation of the turbine blades? Are the blades located within their own cylindrical embedded region?

BKaiser April 17, 2013 20:46

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

ryancoe April 17, 2013 21:21

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.

BKaiser April 19, 2013 14:19

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?

kyle April 19, 2013 15:20

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.

BKaiser April 19, 2013 15:38

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

kyle April 19, 2013 15:49

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.

malfrienz August 1, 2013 20:47

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.


All times are GMT -4. The time now is 06:28.