CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   precise water / air boundary (http://www.cfd-online.com/Forums/cfx/106112-precise-water-air-boundary.html)

heinz August 19, 2012 10:16

precise water / air boundary
 
I just succeeded in doing the 2d bump tutorial.

Now, I would like to calculate a more precise water / air boundary. At the moment, it looks like a continuum over 4 mm height.

I would appreciate some hints on the relevant parameters. I already increased the max number of refinement steps in the mesh adaption menu of cfx pre. This didn't give any significant change.

Cheers

Heinz

ghorrocks August 19, 2012 19:20

The best way to improve resolution of the free surface is to use a finer mesh in the region of the free surface. I prefer a fine fixed mesh and adaptive mesh refinement has never worked for me with free surfaces very well.

evcelica August 21, 2012 21:41

Not sure on this, but I seem to remember using a specified blend factor of 1 will aid in separating the two fluids more precisely (less smearing) since it is true second order; feel free to call my bluff anyone.....
Glenn is absolutely correct though, as usual, a finer mesh will of course give you finer resolution.

pavitran August 22, 2012 04:04

Quote:

Originally Posted by evcelica (Post 378074)
Not sure on this, but I seem to remember using a specified blend factor of 1 will aid in separating the two fluids more precisely (less smearing) since it is true second order; feel free to call my bluff anyone.....
Glenn is absolutely correct though, as usual, a finer mesh will of course give you finer resolution.

The volume fraction equation uses high resolution scheme, unless the global advection scheme is set to upwind.

More information on this can be found in CFX Modeling guide --> Advection scheme.


I would like to know, What is the effect, when the partition (while solving in parallel mode) lies along the Free surface?

Sometimes, I have observed that the solver crashes due to build up of unphysical values of Eddy viscosity at the partition zone.

ghorrocks August 22, 2012 06:45

I'll call your bluff Erik :)

For free surface models you should use the default compressive scheme for the volume fraction equation. This scheme is specifically designed to capture sharp interfaces and no other schemes will work well at all. For the momentum equations use whatever scheme is sensible - hybrid (with a large blend factor) or high res are the normal choices.

You should try to avoid havign partition boundaries lying along the free surface. This can cause convergence difficulties. You might need to define a partitioning algorithm to avoid this happening.

evcelica August 23, 2012 22:40

Yeah, I don't know where I heard that. I thought a read it somewhere but it was a long time ago. Thanks for correcting me.


All times are GMT -4. The time now is 06:59.