## Fluids

#### Symmetric Model – Asymmetric flow

• shehab Gamrah
Subscriber

I modelled a symmetric geometry with a velocity inlet and two identical pressure outlets, and my problem is I expected flow to be symmetric as model is symmetric but actually the flow becomes asymmetric and depends on Mesh size. In the 2 figures below when I altered the mesh size, the velocity pattern shifted from the upwards channel to the downwards channel hence I would like to know the mesh size shifts the flow pattern and also how can I obtain a symmetrical solution

• Rob
Ansys Employee
Simple answer is you can't. Read up on flow separation, Coanda effect, unconstrained jets and pitchfork bifurcation. You may also want to have a look at how fluidic devices work, mainly the switches. The above results look about as I'd expect, and if you ignore which outlet is used the flow looks pretty much identical in both cases. n
• shehab Gamrah
Subscriber
Thanks Mr RobnBut what seems confusing is that I modelled same geometry but just added a porous medium in the ellipse shaped part and the same boundary conditions and the flow became symmetrical for that case. So I have got 2 questions:n1) Would flow pattern be symmetrical in real life for the previously attached cases or does the coanda effect happen not in only for CFD but in real life.n2) Why is the same case with a porous medium behave in a syemmetric flow manner and the other cases attached above didn't nn
• DrAmine
Ansys Employee
Coanda is real and happens outside CFD too.n
• DrAmine
Ansys Employee
With porous media you are adding resistance and so a sort of smoothing of velocity might happenn
• Rob
Ansys Employee
In the porous case you don't have much (if any) flow in the chamber. Jet hits the surface and then spreads so there's nowhere for it to go to create the asymmetry. n
• shehab Gamrah
Subscriber
Thanks for all the help. I just wanted to raise another question to close the topic. I modelled the same geometry in 3d and done the simulation with same boundary conditions but the flow seems to be symmetrical for the 3d model under the same inlet velocity. so does coanda not occur for 3d models or should I increase velocity for 3d case and the flow would become asymmetrical.nn
• DrAmine
Ansys Employee
Coanda occurs in 3D, 2D and 1D. You can even run transient and create a mean of flow to check if it is chaning.n
• Rob
Ansys Employee
That jet looks to diffuse quite quickly, how well resolved is it? Fluidic switches take advantage of this phenomena, and if you nudge the jet one way or the other you can control the outcome. In my opinion the best use of this was in the US:they had a rocket powered shopping trolley at (I think, it's been a while since I worked in this field) Harry Diamond Labs in the US. n
• shehab Gamrah
Subscriber
Dear Mr RobnSo i've done a mesh convergence study on the case and still the flow is symmetric and not similar to the 2d case. Is there any way I can resolve this issue to obtain an asymmetric flow similar to the 2d case.n
• Rob
Ansys Employee
Please can you post some images? Velocity & pressure on the mid plane same view as before. Zoom in around the expansion area. n
• shehab Gamrah
Subscriber
nnThe 1st image is velocity, 2nd is pressurenn
• Rob
Ansys Employee
Run that on, I think you'll find it'll switch in a bit. If Fluent is hitting the convergence criterion turn off Checking in the Monitor-Residual panel. n
• DrAmine
Ansys Employee
The velocity image is telling me that is still developing. Again in 3D you should quantify it from other planes as the might be in plane but deviated.n