CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Rotating boundary (http://www.cfd-online.com/Forums/cfx/23979-rotating-boundary.html)

eros May 14, 2007 10:50

Rotating boundary
 
Hello! I've to carry out a calculation in which a rotating boundary is present.The boundary moves into the fluid domain at a constant angular velocity.I set up an unsteady calculation in which boundary rotation around x axis is defined with a CEL like this:

omega = 890 [rad s^-1] alfa=omega * t sy = ((y*cos(alfa))-(z*sin(alfa)))-y sz = ((y*sin(alfa))-(z*cos(alfa)))-z

CFX solver gives me always the same error, that is: "A negative element volume has been detected..." Time step is very small (about 10^-5). I tried different meshes and different definitions for mesh stiffness but I obtained always the same result. Thank you for collaboration, bye!


Glenn Horrocks May 14, 2007 18:26

Re: Rotating boundary
 
Hi,

1) If you are doing rotation then use the rotating frame of reference model rather than a general moving mesh.

2) If you use moving mesh through CEL to define your motions you might be limited in how far you can rotate. If you use specified displacement on the boundaries the default mesh smoothing algorithm for the interior nodes will definitely fail and cause negative volume elements. The way to fix this is to define a subdomain in the rotating region and specify the mesh motion in the entire subdomain. This means you have to describe the motion at all points by a CEL function which is not always possible.

3) To debug mesh motion simulations, use the expert parameters to turn the fluid, turbulence, heat and any other equations off and output a transient result file each iteration. This should run quickly as it has no flow variables to solve for. You can then view the progress of the mesh motion in CFX-Post and see exactly where the mesh is going wrong.

Glenn Horrocks

eros May 15, 2007 03:21

Re: Rotating boundary
 
Hi Glenn, thanks a lot for your response! You mean that I've to define a rotating subdomain?Actually rotating boundaries are closing an empty space, have I define a solid subdomain!? I'm not sure to have understood your hint. Thanks again, bye!

Glenn Horrocks May 15, 2007 18:33

Re: Rotating boundary
 
Hi,

Can you describe what you are modelling? Then I might be able to be more specific.

Glenn Horrocks

eros May 16, 2007 04:02

Re: Rotating boundary
 
I have to simulate the effect of the air on a crankweb profile. The crankweb rotates in a mixtur of air and oil. In practice it is a solid body on shaft which rotates into a fluid domain. How can I sent you some images to explain the problem in a better way?

Glenn Horrocks May 16, 2007 18:09

Re: Rotating boundary
 
Hi,

I would have thought this was easily modelled using a rotating frame of reference. Put the crank in a RFR, the crank case in a stationary frame of reference and join the two with a GGI. Forget about the mesh motion, it will not work here.

Glenn Horrocks


All times are GMT -4. The time now is 19:24.