[ar_mofidi]

Hi guys

I want to know that, how can I use icoFoam for the laminar microchannel and which of the boundary condition need to use, periodic or inlet/outlet.

Thanks,

[wenterodt]

If you want to simulate a fully developed channel flow in constant cross sections or in a periodically repeating geometry, the cyclic boundary condition for the U-field is what you need. The easiest way to prescribe a pressure drop between inlet and outlet is to use the fan-boundary condition. I.e. in constant/polyMesh/blockMeshDict use e.g.

cyclic inout
  (
    (4 7 3 0)
    (6 5 1 2)
  )

Then in 0/U

  inout
  {
    type cyclic;
    value uniform (0 0 0);
  }

In 0/p write

inout
  {
    type fan;
    patchType cyclic;
    f List<scalar> 1(-0.005); // p_OF = p_real / rho
    value uniform 0;
  }

and mind that the OpenFOAM pressure is divided by the density in incompressible flow. The pressure drop (here 0.005*rho) that is needed for a certain mean velocity can be calculated by the Poisseuille number (if available) or must be guessed and then corrected. (Yes, I know there is channelFoam, but I cannot recommand that for various reasons.)
Here the "value"-entries are only used for the first iteration (and to prevent paraFoam from crashing) and are then overwritten.
Good luck!

[Thomas Baumann]

Hi,

an other way is to use mapped boundary condtions.

http://www.cfd-online.com/Forums/ope...condition.html

Regards Thomas

[ar_mofidi]

Originally Posted by wenterodt

If you want to simulate a fully developed channel flow in constant cross sections or in a periodically repeating geometry, the cyclic boundary condition for the U-field is what you need. The easiest way to prescribe a pressure drop between inlet and outlet is to use the fan-boundary condition. I.e. in constant/polyMesh/blockMeshDict use e.g.

cyclic inout
  (
    (4 7 3 0)
    (6 5 1 2)
  )

Then in 0/U

  inout
  {
    type cyclic;
    value uniform (0 0 0);
  }

In 0/p write

inout
  {
    type fan;
    patchType cyclic;
    f List<scalar> 1(-0.005); // p_OF = p_real / rho
    value uniform 0;
  }

and mind that the OpenFOAM pressure is divided by the density in incompressible flow. The pressure drop (here 0.005*rho) that is needed for a certain mean velocity can be calculated by the Poisseuille number (if available) or must be guessed and then corrected. (Yes, I know there is channelFoam, but I cannot recommand that for various reasons.)
Here the "value"-entries are only used for the first iteration (and to prevent paraFoam from crashing) and are then overwritten.
Good luck!

Dear Tammo

thanks for your help. but, I have some other questions. could you tell me, what is the Fan-boundary condition and is it possible to use this B.C in icoFoam. also, I want to know for laminar channel flow, can I use icoFoam?