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!

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

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!

Hi,

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

Glenn Horrocks

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?

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