[ericnutsch]

After mesh generation, i would like to change the angle of attack of the flow field. This is doable with a diamond or square mesh with separate outlet and inlet boundaries.

However to increase mesh quality i would like to use a "C" mesh or an "O" mesh. The curved boundaries however demands for a single boundary to handle both inlet and outlet.

Can open foam do this? What would be the boundary type/name?


Every bit helps, Thanks guys!

[AlanR]

Eric,

There's a derived boundary type called inletOutlet (and another called outletInlet) that switches between a velocity inlet and a pressure outlet depending on the direction of U - there's a little more information in the User Guide. I've seen it in other threads, so you could search the forum for more information. If you divided the O shaped domain into two or more sections, the inletOutlet boundary will probably work. I haven't tried it (yet). Good luck,

Alan

[ericnutsch]

Hey Alan,

"inletOutlet" huh, doesnt get more self explanatory than that.

No matter how many times i read that userguide i never seem to take it all in...

Do you think inletOutlet and outletInlet are different or just calls to the same function? I guess i will have to mess around with them a bit.


Thanks Alan!

[maddalena]

Hello Eric,
I used the inletOutlet boundary condition for a case similar to yours, see here. Scrolling the different posts you can see what the effects of imposing wrong boundary conditions for a spherical domain are.

As for you, I would suggest:

• inletOutlet boundary conditions for U, k and epsilon,
• zeroGradient for p,

at the external domains.
Hope that helps.
Cheers,
Maddalena.

[ericnutsch]

I am attempting to implement inletOutlet on a single boundary mesh using the skeleton files of the airfoil2d tutorial. When i try running simpleFoam it says "Starting time loop" and does nothing. Obviously I have specified the boundary conditions incorrectly, but I am not sure what they might be or where to find them. The airfoil2d tutorial used freestream on the inlet and outlet.

freestream is to inletOutlet
as frestreamValue is to ___________
& as freestreamPressure is to _____________

I found some pages in Doxygen but they were unhelpful to me.
http://foam.sourceforge.net/doc/Doxy...atchField.html
http://foam.sourceforge.net/doc/Doxy...atchField.html


It may be possible that I could figure out the required values from the source code, but I am uncertain where to look... thoughts?

[ericnutsch]

Thanks maddalena, your post was very helpful.

When using the airfoil2d tutorial case files:
freestream is to inletOutlet
as frestreamValue is to inletValue
& as freestreamPressure is to inletOutlet; inletValue uniform 0;

Works great!



Once I get a little more comfortable with it i will test the difference between inletOutlet and outletInlet.

Thanks again