# Material interfaces and the laplacian operator

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

 November 7, 2006, 09:35 Hi to all I am fairly new to #1 Member   Ivor Clifford Join Date: Mar 2009 Location: Switzerland Posts: 91 Rep Power: 10 Hi to all I am fairly new to OpenFoam so if anyone could help me, I'd appreciate it. I am solving a simple diffusion equation of the form fvm::laplacian(gamma,phi) == Src How does one implement an effective gamma at a face separating two cells with different gamma values (i.e. different materials). This would be done for any solid heat conduction problem (where an interface between solid materials of different conductivities exists). As I understand it, it is necessary to define an interpolation scheme and add a weighting parameter to the laplacian operator. Could somebody please clarify how this is done practically in OpenFOAM, or at least point me to an example where this is done. Thankyou in advance

 November 7, 2006, 10:03 I think the answer is in the s #2 Senior Member     Dragos Join Date: Mar 2009 Posts: 649 Rep Power: 13 I think the answer is in the solver written by Daniele Panara, and presented in : conjugateHeat

 November 7, 2006, 10:30 When you specify the Laplaciam #3 Senior Member   Hrvoje Jasak Join Date: Mar 2009 Location: London, England Posts: 1,810 Rep Power: 25 When you specify the Laplaciam scheme in a dictionary, you will have something like this: laplacian(nu,U) Gauss linear corrected; The word "linear" here tells you how to interpolate nu between the cell centres. The final word,"corrected", tells you how to calculate the surface-normal gradient needed by the operator - this one is corrected for mesh non-orthogonality. Other choices for the interpolation scheme can be made here, for example "harmonic" or any other scheme. Keep in mind that more complex schemes may requre more than one word, i.e. you may have additional parameters before the snGradScheme. Enjoy, Hrv sh.d likes this. __________________ Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk

 November 7, 2006, 11:06 Hi, Thankyou for your respons #4 Member   Ivor Clifford Join Date: Mar 2009 Location: Switzerland Posts: 91 Rep Power: 10 Hi, Thankyou for your response. The method proposed there would work but it seems to me to be unnecessary to define a new mesh for each new material. I was thinking more along the lines of updating the face conductivities, so that when openFOAM calculates k*grad(T) at the face, the k value used is not a linearly interpolated value but rather a custom calculated value. This value would depend on the P and E cell conductivity values and the distance of each cell centre to the face. k=(dx_E+dx_P)*k_P*k_E / (dx_P*k_E + dx_E*k_P)

 November 7, 2006, 11:15 Thanks Hrv Seeing the equatio #5 Member   Ivor Clifford Join Date: Mar 2009 Location: Switzerland Posts: 91 Rep Power: 10 Thanks Hrv Seeing the equation a gave in my last post, do you know if FOAM has a suitable scheme built in. Where will I find a list of the available schemes? Regards Ivor

 November 7, 2006, 11:31 Looking at your scheme, it loo #6 Senior Member   Hrvoje Jasak Join Date: Mar 2009 Location: London, England Posts: 1,810 Rep Power: 25 Looking at your scheme, it looks to me like harmonic interpolation. If you wish to implement your own interpolation, I've got a Laplace operator for you that will take the diffusivity as a surfaceScalarField, i.e. you can do the face interpolation beforehand in the code and present the face values directly. Hrv __________________ Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk

 November 8, 2006, 03:17 Thanks Hrv The laplace operat #7 Member   Ivor Clifford Join Date: Mar 2009 Location: Switzerland Posts: 91 Rep Power: 10 Thanks Hrv The laplace operator that will take the diffusivity as a surfaceScalarField sounds ideal. could I get that from you? Regards Ivor

 November 8, 2006, 07:36 You mis-understood me: the ope #8 Senior Member   Hrvoje Jasak Join Date: Mar 2009 Location: London, England Posts: 1,810 Rep Power: 25 You mis-understood me: the operator is already in the library so you don't need any code from me. Hrv __________________ Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk

 November 8, 2006, 09:57 Right you are Hrv: I had anoth #9 Member   Ivor Clifford Join Date: Mar 2009 Location: Switzerland Posts: 91 Rep Power: 10 Right you are Hrv: I had another look at the doxygen documents and I see the operator you're talking about. Will give it a try... thanks Ivor

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post liuhuafei OpenFOAM Running, Solving & CFD 6 October 3, 2009 06:58 Pablo FLUENT 1 January 25, 2007 11:54 seyed Farid hosseinizadeh FLUENT 0 December 17, 2006 22:56 cliffoi OpenFOAM 0 November 6, 2006 11:42 J. Park FLUENT 0 September 17, 2003 12:39

All times are GMT -4. The time now is 20:54.