# Periodic B.C or Inlet/Outlet B.C

 Register Blogs Members List Search Today's Posts Mark Forums Read

 February 24, 2010, 07:41 Periodic B.C or Inlet/Outlet B.C #1 New Member   alireza Join Date: Apr 2009 Location: iran Posts: 11 Rep Power: 16 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, Luttappy likes this.

 February 25, 2010, 01:19 #2 New Member   Tammo Wenterodt Join Date: Mar 2009 Posts: 24 Rep Power: 16 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. Code: ```cyclic inout ( (4 7 3 0) (6 5 1 2) )``` Then in 0/U Code: ``` inout { type cyclic; value uniform (0 0 0); }``` In 0/p write Code: ```inout { type fan; patchType cyclic; f List 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! sunliming, arvindpj, mgg and 2 others like this.

 February 25, 2010, 03:58 #3 Member   Join Date: Apr 2009 Location: Karlsruhe, Germany Posts: 98 Rep Power: 16 Hi, an other way is to use mapped boundary condtions. http://www.cfd-online.com/Forums/ope...condition.html Regards Thomas sunliming likes this.

February 27, 2010, 03:36
#4
New Member

alireza
Join Date: Apr 2009
Location: iran
Posts: 11
Rep Power: 16
Quote:
 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. Code: ```cyclic inout ( (4 7 3 0) (6 5 1 2) )``` Then in 0/U Code: ``` inout { type cyclic; value uniform (0 0 0); }``` In 0/p write Code: ```inout { type fan; patchType cyclic; f List 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?