
[Sponsors] 
August 31, 2010, 10:51 
Adding acceleration term in icoDyMFoam

#1 
Senior Member
Pavan
Join Date: May 2009
Location: Melbourne
Posts: 101
Rep Power: 8 
Hey guys, real simple question. My moving reference frame is accelerating 0.5*pi*A*T*sin(2*pi*t/T) in xdirn and sqrt(3)/2*pi*A*T*sin(2*pi*t/T) in ydirn. A, T, pi are constants, t is time. I'm trying to add these to the momentum equation but it doesn't compile. Here's what I've got:
Ueqn.H Code:
volScalarField pi = 3.1415926535897932384626433832795028841971693993751; volVectorField acc = pi*0.1091911*sin(2*pi*runtime.time().value()/1.091911)*(0.5*vector(1,0,0)+pow(3,0.5)*vector(0,1,0)); fvVectorMatrix UEqn ( fvm::ddt(U) + fvm::div(phi, U)  fvm::laplacian(nu, U)  acc ); if (momentumPredictor) { solve(UEqn == fvc::grad(p)); } 

September 1, 2010, 11:32 

#2 
Senior Member
Pavan
Join Date: May 2009
Location: Melbourne
Posts: 101
Rep Power: 8 
Ok....put it this way,
1. How can I create an empty volScalarField with dimensions acceleration? 2. How do I introduce the runtime class into Ueqn.H? (What header file do I need to introduce) I couldn't find any of this basic stuff in the programmer's guide... 

September 1, 2010, 16:41 

#3 
New Member
Ozgur Kirlangic
Join Date: May 2009
Location: Istanbul
Posts: 16
Rep Power: 8 
Hi Pavan,
I am not expert but if I make some comments on your code, I can say that: 1. I wouldn't define pi as volScalarField, because it is a constant scalar, not a field variable which has different values in time and space. So I think, Code:
scalar pi 3.1415926535897932; There might (/or not) also be an already defined macro for the number pi in OpenFOAM but I haven't used it before. 2. I wouldn't define acc as volVectorField neither (if I won't need to use it over and over, or do other calculations with it). Because, if you want to define a volVectorField, then (as far as I understood up to now) then also you will need to construct an IOobjet and make mesh association, defining the dimensions etc., such as: Code:
volVectorField acc ( IOobject ( "acc", runTime.timeName(), mesh, IOobject::NO_READ, IOobject::AUTO_WRITE ), mesh ); What can be done may be writing the acc formula directly into the Ueqn. However, I am not sure about how will the expressions like 0.5*vector(1,0,0) compiled. They might need to be verified separately. 3. I haven't used icoDyMFoam so I don't know anything about it, however, I have been using interDyMFoam for a while and I guess the "DyM" stands for dynamic mesh (and it maybe the same in icoDyMFoam). In interDyMFoam the mesh movement is imposed by an additional utility called gen6DoF, which is in turn equivalent to an extra acceleration term to UEqn. Since your acceleration term is also only a function of time, and is independent of space, use of gen6DoF explicitly might also be considered. Regards, Ozgur 

September 1, 2010, 17:43 

#4 
Member
Simon Lapointe
Join Date: May 2009
Location: Québec, Qc, Canada
Posts: 33
Rep Power: 8 
Hi Pavan,
Since your source term is constant in space you don't need to define a volVectorField, a simple vector would do it. You could try something like: Code:
dimensionedVector accX ( "accX",dimensionSet(0, 1, 2, 0, 0),vector(1, 0, 0) ); dimensionedVector accY ( "accY",dimensionSet(0, 1, 2, 0, 0),vector(0, 1, 0) ); scalar Pi = mathematicalConstant::pi; dimensionedVector acc = Pi*0.1091911*sin(2*Pi*runTime.value()/1.091911)*(0.5*accX+pow(3,0.5)*accY); 

September 1, 2010, 18:37 

#5 
Senior Member
Pavan
Join Date: May 2009
Location: Melbourne
Posts: 101
Rep Power: 8 
Thanks, Ozgur!
1. Agreed about the scalar pi thing. 2. I don't know I was referring to this thread: Rotating Reference Frame (3rd post by Henry) where Fcent is defined as a volVectorField without being a field variable. 3. Yeah icoDyMFoam is just the dynamic mesh version of icoFoam, the incompressible fluid solver with no turbulence. 

September 1, 2010, 18:41 

#6 
Senior Member
Pavan
Join Date: May 2009
Location: Melbourne
Posts: 101
Rep Power: 8 
Also, thanks Simon! Will try this asap


September 4, 2010, 12:18 

#7 
Senior Member
Pavan
Join Date: May 2009
Location: Melbourne
Posts: 101
Rep Power: 8 
Well, with the extra help of an experienced OF user I got the following to compile:
Code:
scalar Pi = mathematicalConstant::pi; dimensionedScalar accCt("accCt",dimensionSet(0,1,2,0,0,0,0),10000*Foam::cos(2*Pi*runTime.value()/0.5)); dimensionedVector acc("acc",dimensionSet(0,1,2,0,0,0,0), vector::zero); acc.component(vector::X) = 0.5 * accCt; acc.component(vector::Y) = 0.5 * Foam::sqrt(3.0) * accCt; fvVectorMatrix UEqn ( fvm::ddt(U) + fvm::div(phi, U)  fvm::laplacian(nu, U) ); solve(UEqn == accfvc::grad(p)); 

September 18, 2010, 23:07 

#8 
Senior Member
Pavan
Join Date: May 2009
Location: Melbourne
Posts: 101
Rep Power: 8 
I notice in dnsFoam the force term is implemented like so:
Code:
fvVectorMatrix UEqn ( fvm::ddt(U) + fvm::div(phi, U)  fvm::laplacian(nu, U) == acc ); solve(UEqn == fvc::grad(p)); Code:
fvVectorMatrix UEqn ( fvm::ddt(U) + fvm::div(phi, U)  fvm::laplacian(nu, U) ); solve(UEqn == (accfvc::grad(p))); 

September 18, 2010, 23:54 

#9 
Senior Member

They are different.
In the first, acc is introduced to momentum equation, and in the second acc was introduced into pressure equation and pressure equation should also be altered accordingly (if you don't include acc relative term in pressure, the results should differ much). If acc has effect on the velocity, doing in the second way is more implicit. please see derivation of pressure equation in Henrik Rusche's phd thesis. regards, Junwei 

September 20, 2010, 11:43 

#10 
Senior Member
Pavan
Join Date: May 2009
Location: Melbourne
Posts: 101
Rep Power: 8 
Thanks for the reply Su Junwei! So I take it the first approach is valid but not as implicit as the second approach (with modification to the pressure equation)?


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
ATTENTION! Reliability problems in CFX 5.7  Joseph  CFX  14  April 20, 2010 15:45 
Adding implicit source term to momentum equation  fs82  OpenFOAM  6  September 23, 2009 03:29 
Adding a momentum source term  segersson  OpenFOAM Running, Solving & CFD  5  March 3, 2006 00:06 
adding souce term  cfp  CFX  0  July 14, 2002 10:43 
adding source term confusion  tedmcc  CFX  4  September 27, 2001 05:05 