
[Sponsors] 
May 7, 2012, 17:07 
Solving a nonhomogeneous wave equation (FWH)

#1 
New Member
Wouter
Join Date: Mar 2012
Posts: 6
Rep Power: 6 
Dear all,
I am trying to build a solver which solves a nonhomogeneous wave equation. You may ask, why such a solver? It is used for solving a simplified version of the Ffowcs Williams Hawkings differential equation, used in aeroacoustics. To be specific, I would like to use Curle's analogy, and only consider the pressure perturbation at the wall. Therefore I wrote some code which extracts the pressure at the boundary, I multiply it with the normal outward vector, and taking the divergence of the volVectorField (which is zero in the internal field, and has values in the boundary field) to create a volScalarField. Next, I forced this last volScalarField to be zero in the internal field (initial there were some values because of the corners of the geometry) Now the next step is to solve the wave equation throughout the domain, with the source term as indicated above. I started by simply using the following relation: solve((fvm::d2dt2(rhoPrimeCurle)  c0 * c0 * fvm::laplacian(rhoPrimeCurle)== CurleTerm)); However, due to the fact that the source term only consist of values at the wall, no solution can be obtained. There are 0 iterations required to solve this. I am thinking this is because of the fact that the internalField = 0. Therefore, I would like to fill the CurleTerm.internalField() somehow by interpolating the values from the boundary to the nearest cells. Is there anyone who has some experience with this method, or perhaps, is there anyone with a brilliant idea how to omit this. I assume someone tried to implement the FWH equation before in OF. Many thanks in advance 

May 7, 2012, 17:22 

#2 
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,720
Rep Power: 28 
Hi
There is a minor detail, which is unclear to me. You say that you generate a surfaceVectorField, where you only populate the boundary values with values different from vector::zero. These values are bcpressure times the face normal. Here is the question: How does the divergence of that field end up with a zero internal field? Those cells adjacent to the boundary must have nonzero values, since the boundary faces themselves are nonzero, whereas the internal faces equal vector::zero. Maybe you should try applying the divergence of your volVectorField in your wave equation; at least this provides you with a nonhomogeneous source term. Kind regards, Niels 

May 8, 2012, 04:44 

#3 
New Member
Wouter
Join Date: Mar 2012
Posts: 6
Rep Power: 6 
Dear Niels,
Thank you very much for your quick reply. I will try to clarify some things now. First of all, I indeed only copy the values from the wall patch to a new volVectorField like this: pB.boundaryField()[wallID] = p.boundaryField()[wallID].patchInternalField()*(mesh.Sf().boundaryField()[wallID] /mesh.magSf().boundaryField()[wallID]); where the last term between the ( ) simply indicates the outward normal vector. Now I will have an empty internal field, and only vectors of the boundary patch called "wall" (since wallID finds the patchID "wall"). Next, I calculate the dipole source term for the wave equation: CurleTerm = rho * fvc::div(pB); Indeed, as you already mentioned in your post, this results in some nonzero values in this volScalarField "CurleTerm". However, in my opinion these inner values are useless, since they only appear at the corner of meshes, i.e. where the normal outward vector of the adjacent is not simply (1 0 0). Therefore, afterwards i force the internalField to be zero, i.e. CurleTerm.internalField() = 0; I will now end up with a volScalarField, which is completely empty in the internalField but contain values at the boundary patches. This is also what I want, since the source term analytically contains a dirac delta function which is only 1 on the surface. Equating the source term to the wave equation results in a homogeneous wave equation without source term... Somehow, when solving a PDE, only the values of the internalField are used, and not the values at the boundary patch. Therefore I am now looking to some kind of script which translate the boundary values in the boundary patch, to the adjacent cells in order to solve for the density in the wave equation. 

May 8, 2012, 04:57 

#4 
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,720
Rep Power: 28 
OK. I am not sure that I understand the motivation to clear the divergence field, but never mind. You could e.g. do the following to copy boundary values to internal values:
Code:
labelList count( CurleTerm.internalField().size(), 0 ); forAll( mesh.boundary(), patchi ) { if ( WALL TYPE) { const labelList & fc( mesh.boundary()[patchi].faceCells() ); const scalarField & ctw( CurleTerm.boundaryField()[patchi] ); forAll( ctw, facei ) { CurleTerm[fc[facei]] += ctw[facei]; count[fc[facei]]++; } } } forAll( count, celli ) { if ( count[celli] ) curleTerm[celli] /= count[celli]; } Code:
curleTerm.internalField /= count; Niels 

August 24, 2016, 03:41 

#5 
Member
Ahmad Habib
Join Date: Nov 2014
Location: Aleppo, Syria
Posts: 34
Rep Power: 4 
Dear wcpvandervelden,
I saw your work "Numerical investigation of an upper airway in a patient suffering from stridor" and I wounder If you can share your solver, I'm interested in this field. Regards. 

Tags 
boundary interpolation, curle, fwh 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Calculation of the Governing Equations  Mihail  CFX  7  September 7, 2014 06:27 
Upgraded from Karmic Koala 9.10 to Lucid Lynx10.04.3  bookie56  OpenFOAM Installation  8  August 13, 2011 04:03 
Error while running rhoPisoFoam..  nileshjrane  OpenFOAM Running, Solving & CFD  8  August 26, 2010 12:50 
Problems with simulating TurbFOAM  barath.ezhilan  OpenFOAM  13  July 16, 2009 05:55 
Differences between serial and parallel runs  carsten  OpenFOAM Bugs  11  September 12, 2008 11:16 