I have been experiencing a high degree of numerical diffusion when I run combustion in CFX on a hybrid tet/prism mesh, specifically numerical diffusion with the turbulence transport equations when the flamefront comes within the vacinity of the tet/prism boundary. It seems as if CFX has difficulty resolving the shear layer when a region of flow with a high shear strain gradient comes near the inflated boundary.

I have tried varying turbulence schemes, advections schemes, stress and turbulence diffusion schemes, mesh refinements, etc... but nothing seems to alleviate the problem. Has anyone encountered the this type of behavior before or have any ideas what else I might try to mitigate this false diffusion?

Thanks

John

How quickly does the mesh expand from the last prism and first tet? The volume ration should be between .5 and 2.

-CycLone

Also what differencing scheme are you using? Need a second order scheme.

Glenn Horrocks

I've varied the differencing scheme. I usually run using high resolution. CFX uses the first order upwind scheme by default for turbulence but I changed the CCL to run them high res as well. Post processing the beta values for k and omega so that within the inflated boundary near the wall they are nearly fully second order; however, about half way through the inflated boundary it drops suddenly to first order and then spikes back to second order. I've tried specifying the blend factor but specifying beta > 0.5 causes the solution to become very unstable and crash.

Hi,

You probably need a very good quality grid in this local area to allow you to run at second order differencing. Can you do a local high-quality hex grid? Maybe just do a simple test case to see if this helps. Also don't forget the mesh expansion ratio Cyclone talked about, for a high quality grid keep it below 1.05.

Glenn Horrocks