[Raymond.Leoi]

I try to set up a translational periodic boundary condition. Any idea on how to specify it and set up pressure gradient?

Cheers,
Raymond

[cfdonline2mohsen]

I quote the user guide section 5.2.2 Base types :

cyclic: Enables two patches to be treated as if they are physically connected; used for repeated geometries, e.g. heat exchanger tube bundles. One cyclic patch is linked to another through a neighbourPatch keyword in the boundary file. Each pair of connecting faces must have similar area to within a tolerance given by the matchTolerance keyword in the boundary file. Faces do not need to be of the same orientation.

thus cyclic b.c. can be specified using:

type cyclic;

in the blockMesh. have a look at the section 5.3.1.4 of the user guide in: 5.3.1 Writing a blockMeshDict file
I quote it again:

When specifying a cyclic patch in blockMesh, the user must specify the name of the related cyclic patch through the neighbourPatch keyword. For example, a pair of cyclic patches might be specified as follows:

left
type cyclic;
neighbourPatch right;
faces ((0 4 7 3));

right
type cyclic;
neighbourPatch left;
faces ((1 5 6 2));

and then in the 0 folder for the desired quantities use the cyclic keyword.

you can explain your case in detail for further help!

[Raymond.Leoi]

Let's say the case is the fully-developed laminar flow in a pipe, where the outlet is the same to the inlet. In general, we can specify the velocity or the pressure gradient. Is it clear to you?

[mohammad81]

Thanks for your good comment.
I am new to OpenFOAM, so forgive my simple question.
1. I did not understand; shall we write this cyclic commands:

left
type cyclic;
neighbourPatch right;
faces ((0 4 7 3));

right
type cyclic;
neighbourPatch left;
faces ((1 5 6 2));


"in blockMeshDict" file or "boundary" file? since I think the format you entered here seems to be for boundary, but it is said that it is for blochMeshDict.
2. What shall we also write for U and P conditions? something like this:

for p:
type: cyclic
value: uniform 0


for U:
type: cyclic
value: uniform (0 0 0)

Thanks again.

[jptorol]

Dear mohammad81:

Generally speaking write in BlockMeshDict, actually boundary file is an output.
Regards,

JP

[andre.weiner]

Originally Posted by Raymond.Leoi

I try to set up a translational periodic boundary condition. Any idea on how to specify it and set up pressure gradient?

Cheers,
Raymond

Hello,

i was facing the same problem some time ago. Have a look at the channel395 tutorial
.../tutorials/incompressible/pimpleFoam/channel395

There is a fvOption called "pressureGradientExplicitSource" in which the pressure gradient source is calculated by an average velocity. As your problem is translatory, it should work easily. (at least in my mind it works :-)
Keep in mind that currently only the kinematic pressure is handled so that you will get an unphysical static pressure field. If you don't need it for further calculations, it doesn't matter.

Best regards

[lhcamilo]

Indeed you can either follow the example of the channelFoam tutorial, where a constant mass flow is imposed and a pressure gradient correction is applied after each iteration. Or you can set a fixed pressure gradient into the solver, which I reckon is a wee bit more realistic for turbulent flows.

This can be done by adding an entry to the readFields.H file that reads the value of a dimensioned vector (or scalar if you multiply it by a flowDirection vector) that reads the transportProperties file. It goes without saying that you need to add an entry to the transportProperties file as well.

In the momenum equation of the channelFoam tutorial you should have

...
==
flowDirection*gradP };

in case gradP is a scalar and

...
==
gradP };

in case gradP is a vector.

[MaLa]

Hi lhcamilo

I tried modifying the simpleFoam solver to have a constant pressure gradient whose magnitude is equal to -1 (i.e. gradP = -1 * flow direction (1 0 0), where gradP is a dimensioned vector which I define in the createFields.H

I added the following lines in createFields.H

Info<< "Reading gradP \n"<<endl;
volVectorField gradP
(
IOobject
(
"gradP",
runTime.timeName(),
mesh,
IOobject::NO_READ,
IOobject::AUTO_WRITE
),
mesh,
dimensionedVector("gradP", dimensionSet(0,1,-2,0,0,0,0), Foam::vector(-1,0,0))
);

Also, I modified my simpleFoam Solver by changing the momentum predictor equation in UEqn.H

// Momentum predictor

tmp<fvVectorMatrix> UEqn
(
fvm::div(phi, U)
+ turbulence->divDevReff(U)
==
fvOptions(U)
);

UEqn().relax();

fvOptions.constrain(UEqn());

// solve(UEqn() == -fvc::grad(p));

solve(UEqn() == -gradP);
fvOptions.correct(U);

Do you think this should do the trick? Do you know if I need to change something in pEqn.H?

[Udvavisk]

Hey Andre, Thanks. I struggled a lot for this.

[GKARIMI]

Hi All,

I am new in OP, I have a rotating object which has axisymmetric feature in a 3D geometry. I modeled it with MRF method, however since it is a large model, it takes a long time to converge, so I want to use symmetry of the geometry and just solve part of the geomtry. I don't know how I should apply cyclic boundary for meshing (blockmesh, snappyHexmesh), I was wondering if anybody could help me. Thank you in advance.