
[Sponsors] 
RotatingWallVelocity Boundary Condition: mathematical and physical explanation? 

LinkBack  Thread Tools  Display Modes 
June 19, 2015, 07:27 
RotatingWallVelocity Boundary Condition: mathematical and physical explanation?

#1 
New Member
Join Date: Jun 2015
Posts: 1
Rep Power: 0 
Dear All Foamers,
I am using the 'rotatingWallVelocity' boundary condition for a rotating device. The description of the boundary condition available in OpenFOAM is; "Replaces the normal of the patch value so the flux across the patch is zero" I would appreciate if someone could explain how this type of boundary condition actually takes place, both from a mathematical point of view and from a physical point of view. In particular, I am curious on how the effect of the boundary condition is reflected on the flow field around the patch. Many thanks in advance! 

November 11, 2015, 23:29 

#2  
Member
methma Rajamuni
Join Date: Jul 2015
Location: Victoria, Australia
Posts: 32
Rep Power: 2 
Quote:
If you look at the rotatingWallVelocityFvPatchVectorField.C file you will see how they have done it mathematically. Usually a boundary condition is updated in the member function updateCoeffs(). Code:
void Foam::rotatingWallVelocityFvPatchVectorField::updateCoeffs() { if (updated()) { return; } const scalar t = this>db().time().timeOutputValue(); scalar om = omega_>value(t); // Calculate the rotating wall velocity from the specification of the motion const vectorField Up ( (om)*((patch().Cf()  origin_) ^ (axis_/mag(axis_))) ); // Remove the component of Up normal to the wall // just in case it is not exactly circular const vectorField n(patch().nf()); vectorField::operator=(Up  n*(n & Up)); fixedValueFvPatchVectorField::updateCoeffs(); } Surface velocity of a cell face, Up = omega * (radius x axis), where radius = (patch().Cf()  origin_). radius x axis, '(patch().Cf()  origin_) ^ (axis_/mag(axis_))' give the direction of the velocity. The they corrected Up if it is not tangential to the surface, by removing the component of Up along the normal direction to the surface. where n.Up (n & Up) give the magnitude along the normal direction. In the physical point of view this is a noslip boundary condition which assume the velocity on the surface of the patch is same as the velocity on the wall. This boundary condition is a nopenetration boundary condition as well since fluid particle do not penetrate to the wall because no flow velocity on the surface normal direction. Best, Methma 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
traction free boundary condition  chandra shekhar pant  Main CFD Forum  0  October 3, 2012 03:20 
airfoil boundary condition  Bounecer  Main CFD Forum  6  June 28, 2010 09:24 
transform navierstokes eq. to eulereq.  pxyz  Main CFD Forum  37  July 7, 2006 08:42 
Boundary Conditions  Jan Ramboer  Main CFD Forum  11  August 16, 1999 08:59 