Hi,

If I specify a continuity source in CFX with 0 kg/s total mass inflow and 0 m/s momentum inflow, does this effectively turn the element where the source is located "off"? By that I mean is the momentum forced to be zero at those locations? If not, can anyone suggest an effective way to force zero velocity at a particular element? Thanks!

- Joshua

"If I specify a continuity source in CFX with 0 kg/s total mass inflow and 0 m/s momentum inflow, does this effectively turn the element where the source is located "off"?"

No - the source is just what you add to the domain. So adding nothing (0 kg/s, 0 momentum) is just like not having a source at all....

For a subdomain, you can use the 'stiff spring' approach to fix velocity values. Look up the word 'Dirichlet' in the CFX help search system - it should come up with a section describing general momentum sources of the form S = -C*(v-v_target). You choose C to be very large, then this source term dominates all other terms at that node, so the solver effectively ends up solving -C*(v-v_target) = 0 in that sub-domain node, and hence you end up with v = v_target in that subdomain. This technique has worked well for me.

I've never seen a way of dealing with an individual element though... I hope others will advise you more.

Good luck. Andy

Thanks for the reply. I just finished verifying your reply regarding the continuity sources. I've already confirmed with CFX help that momentum sources cannot be specified at individual elements. Thanks again.

-- Joshua

Hi Joshua,

What it is it you are trying to accomplish by turning off an element? If you explain your goal, rather than a step you have determined, you may find there is another way altogether.

-CycLone

Hi,

I'm trying to simulate surface roughness in a DNS study of transition over a flat plate affected by surface roughness of a given statistical height, spacing, etc. By turning "off" a few nodes, they become a blockage similar to a roughness element. I've also looked at specifying a source and a source/sink pair to simulate the roughness element. Any other suggestions?

-- Joshua

Hi Joshua,

You should model the roughness in the geometry by creating a pattern and meshing it appropriately.

Note that just turning off an element wouldn't be enough in this case, as you would need more than a single element around the roughness to resolve how the fluid reacts to the roughness. If you intend to do Direct Numerical Simulation, this is the only way, otherwise you are introducing some form of modeling.

Of course if you aren't doing DNS, then the wall roughness option in the turbulence model can do the trick.

-CycLone