[francisco.angel]

Hi, I ran a simulation using simpleFoam of flow over a cylinder. Now I want to obtain force values on the cylinder surface.


So I tried to use the following command:

simpleFoam -postProcess -noZero -func forcesIncompressible

As I read here postProcess functionality in openFOAM 4


Starting with the solver name gives to postProcess utility the field names and stress model. The code fails with the following warning:

--> FOAM Warning : 
    From function Foam::labelHashSet Foam::polyBoundaryMesh::patchSet(const Foam::UList<Foam::wordRe>&, bool, bool) const
    in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 804
    Cannot find any patch or group names matching patch1
--> FOAM Warning : 
    From function Foam::labelHashSet Foam::polyBoundaryMesh::patchSet(const Foam::UList<Foam::wordRe>&, bool, bool) const
    in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 804
    Cannot find any patch or group names matching patch2

I'm unable to find the syntax to specify the patches were I want the force computation to be carried on. Also I don't know why it seems to require 2 patches???


Can someone share any experience with this postProcess function.
Many thanks!

[francisco.angel]

Well, I found the solution after re-reading the manual. So here it is for anyone interested.


For a function like this to work is better to copy the required function file to the system directory, using foamGet

foamGet forcesIncompressible

Then you edit the file on a text editor, in this case changing

patches (patch1 patch2)

to

patches (yourPatch)

And run:

simpleFoam -postProcess -func forcesIncompressible

This will execute without problems.

[uosilos]

how can be done runtime??? (i.e. by including in control dict)

[Krapf]

Copy the content of the file which you get after executing

foamGet forcesIncompressible

into the functions sub-dictionary in controlDict:

...
functions
{
    forces
    {
        #includeEtc "caseDicts/postProcessing/forces/forcesIncompressible.cfg"

        rhoInf      1.225;    // Fluid density
        patches   (patch1 patch2);

        CofR        (0 0 0);
        pitchAxis  (0 1 0);
    }
}