[CST]

Dear All,

as to OpenFOAM version 1.5 there was a boundary condition called 'parabolicVelocity' where parabolic velocity-profiles were applied to patches.

So my question is: Is there any comparable patch-/boundarycondition that can be used?

Or: I got another computation where i can see the parabolic profile in Paraview - how can i export it and use it as inlet-BC for another case?

With best regards,

CST

[AlanR]

CST,

One way to create a parabolic inlet velocity profile is in the tutorials. Look through tutorials/incompressible/simpleFoam/pitzDailyExptInlet. The profile is in the constant/boundaryData/inlet directory. You set up the points file to specify points and the /0/U to set the velocity at each point. I use this method frequently - it's easy to set up. If this doesn't work, you can search the forum for velocity profiles or inlet profiles.

Good luck,

Alan

[fcollonv]

CST,

Another possibility is to use the groovy boundary conditions
see http://openfoamwiki.net/index.php/Contrib_groovyBC

Something like this should make the trick in 2D:

inlet
{
type groovyBC;
variables "yp=pts().y;minY=min(yp);maxY=max(yp);para=-(maxY-pos().y)*(pos().y-minY)/(0.25*pow(maxY-minY,2))*normal();";
valueExpression "10*para";
value uniform (10 0 0);
}

Best regards,

Frederic

[Goutam]

Originally Posted by AlanR

CST,

One way to create a parabolic inlet velocity profile is in the tutorials. Look through tutorials/incompressible/simpleFoam/pitzDailyExptInlet. The profile is in the constant/boundaryData/inlet directory. You set up the points file to specify points and the /0/U to set the velocity at each point. I use this method frequently - it's easy to set up. If this doesn't work, you can search the forum for velocity profiles or inlet profiles.

Good luck,

Alan

Dear Alan

I have simple pipe flow case, length is 1.2 m and radius is = 0.02595 m.
I want to generate the the points file for my case. U(x) = 2U_0 [ 1 - (x/r)^2 ]
x and y varies from -0.02595 to -0.02595 and z varies from 0 to 1.2. Could you give me some suggessions about points file and velocity file in he constant/boundaryData/inlet directory.

Thanks

[sihaqqi]

Alan

Do you have any tutorial for fixing points and velocity. I am a beginner in OpenFoam who is trying to do his MS in CFD. Can you give me a few tips as i have to use 1/7th power law for turbulent flow in my pipe.

Regards