I'm curious if you can have a
 

I'm curious if you can have a cyclic inlet and outlet with the icoFoam solver. I mean, I know you can set the inlet and outlet boundaries as cyclic, but how do you get the fluid to move? Can you set a mass flow rate or pressure gradient? If so, how? I've looked at the channelOodles tutorial case, but haven't figure this out yet.

You can set up a mean velocity
 

You can set up a mean velocity, ubar, instead of mass flow rate or pressure gradient.

Steve

You'll have to use a modified
 

You'll have to use a modified version of icoFoam though. See the channeloodles solver as a source of inspiration.

Sounds like more work than it'
 

Sounds like more work than it's worth to me right now. I'll likely just deal with a entrance region and take my data farther downstream. Thanks.

You could try the directMapped
 

You could try the directMapped boundary condition which recycles sampled data (from inside the domain) to the inlet. See the oodles/pitzDailyDirectMapped case.

hi guys I've tried this in
 

hi guys

I've tried this in a simulation of a channel flow just adding a constant pressure gradient to the icoFoam solver, so modifing the equations. In this way it is possible to work with a dummy pressure that can be cyclic (0 in steady state).
You can take the icoFoam solver folder in /OpenFOAM/applications/solvers/incompressible/icoFoam
copy it and rename as you wish (i used flatChannel). then rename the icoFoam.c as flatChannel.C and add the pressure gradient term as:

fvVectorMatrix UEqn
(
fvm::ddt(U)
+ fvm::div(phi, U)
- fvm::laplacian(nu,U)
+ dpdx
);

in the createField.H you have to add a term that recall a file inside the directory 0 named dpdx. The expression is the same of the call at the p file so you can just modify it.
Then in the 0 directory you have to create a file dpdx similar to the pressure file (remember that the dimensions are different i.e. [0 1 -2 0 0 0]) and set everywhere it constant

also, you have to change the call to the function icoFoam in the directory of the new solvers (follow the pogrammers guide for a better explanation)

i know that is a mess but it worked fine for me in a channel flow. Any suggestions for easier ways are welcome

bye