CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Appropriate boundary conditions for external incompressible flow (http://www.cfd-online.com/Forums/openfoam-solving/60540-appropriate-boundary-conditions-external-incompressible-flow.html)

 mattamos July 27, 2005 11:14

Hi, I'm trying to run simpl

Hi,

I'm trying to run simpleFoam on a test geometry at about M=0.05, laminar. I set up the case using FoamX with an inletOutlet boundary condition in the far-field, but since my flow is external (and there is only one hemispherical patch) this results in the solution converging to a quiescent state.

If I change the 0/U boundary condition to fixedValue the problem becomes overdetermined and never converges.

Is there a more appropriate boundary condition, or a method for specifying a velocity-driven external flow rather than a pressure-driven one?

Thanks,

Matt

 henry July 27, 2005 11:23

What did you choose as the inl

What did you choose as the inletValue for U?

 mattamos July 27, 2005 11:39

Henry, The internalField an

Henry,

The internalField and pressureInletOutletVelocity are both set to uniform (15 0 0).

inletValue is only set for the turbulent fields, which I'm not using at present.

Thanks,

Matt

 henry July 27, 2005 11:45

Try using inletOutlet on U wit

Try using inletOutlet on U with an inletValue of (15 0 0) and zeroGradient on p.

pressureInletOutletVelocity should only be used in conjunction with fixedValue for p which I guess is not appropriate for your case.

 mattamos July 27, 2005 12:22

This results in very large num

This results in very large numbers of iterations for p (about 200 to produce a couple of orders of magnitude drop in the residual) and the solution becomes non-physical after about 20 pseudotime steps.

As I understand it, using zeroGradient for all the boundaries of p (well, there is a symmetry plane, but that is the same thing) means that the matrix is underdetermined?

 henry July 27, 2005 12:25

There is a setReference to han

There is a setReference to handle this and adjustPhi is used to ensure the boundary fluxes obey continuity.

 mattamos July 28, 2005 11:54

Thanks Henry, that seemed to w

Thanks Henry, that seemed to work. I'm still not getting full convergence, but have tracked down the problem to a poor quality element in the boundary region. Hopefully a better mesh will fix that.

 henry July 28, 2005 12:03

You may be able to improve con

You may be able to improve convergence by selecting more stable/lower-order schemes, in partricular you might find it useful to use the limited laplacian. However, improving the mesh is always preferable if possible.

 All times are GMT -4. The time now is 20:27.