[anja]

Hi,

is there a possibility to output the forces a fluid causes on certain walls?

Thanks
Anja

[anja]

Hi again,

or can someone just tell me, whether this option exists at all??

Anja

[eugene]

The posibility doesn't exist as an option, but it is a very simple operation to code. See the lift/drag utility for example.

[anja]

Sorry, but I can't find this utility? Where is it supposed to be?

Anja

[gschaider]

It's missing from the 1.3 distribution (and the folder src/postProcessing that contains the real calculation is missing, too).

Is this by mistake or by design?

[eugene]

Hmm, my mistake.

This code should do the trick though:

pressureForce = vector::zero;
viscousForce = vector::zero;

forAll(patchNames, i)
{
label patchI = mesh.boundaryMesh().findPatchID(patchNames[i]);

if (patchI != -1)
{
vectorField pf =
p.boundaryField()[patchI]
*mesh.Sf().boundaryField()[patchI];

pressureForce += gSum(pf);

vectorField vf =
-mu.boundaryField()[patchI]
*U.boundaryField()[patchI].snGrad()
*mesh.magSf().boundaryField()[patchI];

viscousForce += gSum(vf);
}
else
{
pressureForce += gSum(vectorField(0));
viscousForce += gSum(vectorField(0));
}
}

where patchNames are the names of the boundaries you wish to sum forces for and mu is an effective viscosity field (laminar + turbulent).

[anja]

Hi Eugene,

some more questions:
- where do I get the mu field from?
- do I have to change the code for a compressible fluid?
- where do I have to write the code?
- how can I actually use it?

Thanks alot
Anja

[anja]

Hi all,

maybe someone else can answer my questions?

Moreover I do not know how to write the header, I mean which functions to call.

Thanks
Anja

[msrinath80]

Hi Anja,

I am currently trying to follow instructions given by another user. I have moved back to the 1.2 version. I have no choice. I will give it an try and if everything works fine, I will post the source code and the instructions to get it working. Hope that is fine?

[anja]

Hi you,

that would be great. Thanks.

And maybe you also have an answer to that problem:
I want to multiply the pressure of each face of one patch by it's area, something like p*A (for each face). But how to get A. In te program above it is:
p.boundaryField()[patchI]
*mesh.Sf().boundaryField()[patchI];
I don't how the size of the area is connected with the surface vector.

Anja

[hjasak]

The magnitude of the face area vector is equal to the area. If you don't want the vector, try mesh.magSf(). Quoting from fvMesh.H:


//- Return cell face area magnitudes
const surfaceScalarField& magSf() const;



Hrv

[anja]

Hi pUI,

could you please forward me the instructions from the other user? or do you already have any news? I really need some hints!

Anja

[msrinath80]

Working on it. Will get back to you in a few hours (hopefully).

[anja]

Hi all,

concerning the liftDrag utility.
I can find the following chapter there:

vector Uav = vector::zero;
forAll(U.boundaryField(), patchI)
{
if (U.boundaryField()[patchI].fixesValue())
{
Uav += average(U.boundaryField()[patchI]);
}
}

Why does that not work for p? I tried to compile the changed file and got this error message:

liftDrag2.C:111: error: no match for 'operator+=' in 'pav += Foam::average [with Type = Foam::scalar](((const Foam::UList<foam::scalar>&)((const Foam::UList<foam::scalar>*)(&(+(+ p. Foam::GeometricField<type,>::boundaryField [with Type = Foam::scalar, PatchField = Foam::fvPatchField, GeoMesh = Foam::volMesh]())->Foam::GeometricField<foam::scalar,>::GeometricBou ndaryField:: <anonymous>.Foam::FieldField<foam::fvpatchfield,>: :<anonymous>.Foam::PtrList<t>: :operator[] [with T = Foam::fvPatchField<foam::scalar>](patchI))->Foam::fvPatchField<foam::scalar>::<a nonymous>.Foam::Field<foam::scalar>::<anonymous>.F oam::List<foam::scalar>::<anon ymous>))))'

Thanks for your help.
Anja

[hjasak]

Hi Anja,

I really appreciate the effort you are putting in and the above should work for p with no trouble. I have written the following piece of code which works for me with no trouble - please compare with your stuff and tell me what's the difference:


volScalarField p
(
IOobject
(
"p",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh
);

scalar pav = 0.0;
forAll(p.boundaryField(), patchI)
{
if (p.boundaryField()[patchI].fixesValue())
{
pav += average(p.boundaryField()[patchI]);

}
}

Hrv

[anja]

Hi Hrvoje,
thanks for the answer. Yes I can compile this part, but unfortunately the result is p=0 (at each time step).

Where do I define which patch is to be calculated within the liftDrag utility?

Anja

[hjasak]

That would be because of the if (p.boundaryField()[patchI].fixesValue()) bit.

If you want to do a specific patch, do the findPatchID trick - beware, if there's no such patch, the index returned will be -1.

You can do something like:


label fixedPatchID=aMesh().boundary().findPatchID(myPatc hName);

if (fixedPatchID != -1)
{
// Your stuff here, using
mesh.boundaryMesh()[fixedPatchID];

}


In liftDrag, the force will be calculated for all patches of the wall type:


forAll(patches, patchI)
{
if (isType<wallfvpatch>(patches[patchI]))
{



Hope this helps,

Hrv

[anja]

Hi,
sure your answer helps as usual. But still....

This time I tried:
scalar pav = 0.0;
label fixedPatchID=aMesh().boundary().findPatchID("inlet ");
if (fixedPatchID != -1)
{
forAll(p.boundaryField(), patchI)
{
if (p.boundaryField()[patchI].fixesValue())
{
pav += average(p.boundaryField()[patchI]);
}
}
mesh.boundaryMesh()[fixedPatchID];
}

Error:'aMesh' was not declared in this scope

Moreover I want to come back to the Uavg I have posted before. It does not calculate an average inlet velocity?!

Anja

[hjasak]

Sorry, my mistake: use mesh instead of amesh().

The Uav will sum up the values for all patches that fix the value, which will probably be inlet and all the walls.

Hrv

[anja]

Hi,
it "works" with:
label fixedPatchID = mesh.boundaryMesh().findPatchID("inlet");

But what I got when I use it for one of my cases is:
Time = 50
Reading U
Reading p
Inlet velocity: (1.58209 -0.306071 0)
p : 0
Wall patch 2 named wall :
Reference area: 0.00161926 Reference length: 0.191748 Drag coefficient: 0.0630347

So the wrong inlet velocity and p=0;

Any suggestions?