CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Material interfaces and the laplacian operator

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

Like Tree1Likes
  • 1 Post By hjasak

Reply
 
LinkBack Thread Tools Display Modes
Old   November 7, 2006, 09:35
Default Hi to all I am fairly new to
  #1
Member
 
Ivor Clifford
Join Date: Mar 2009
Location: Switzerland
Posts: 91
Rep Power: 8
cliffoi is on a distinguished road
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
cliffoi is offline   Reply With Quote

Old   November 7, 2006, 10:03
Default I think the answer is in the s
  #2
Senior Member
 
dmoroian's Avatar
 
Dragos
Join Date: Mar 2009
Posts: 647
Rep Power: 11
dmoroian is on a distinguished road
I think the answer is in the solver written by Daniele Panara, and presented in :
conjugateHeat
dmoroian is offline   Reply With Quote

Old   November 7, 2006, 10:30
Default When you specify the Laplaciam
  #3
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
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
hjasak is offline   Reply With Quote

Old   November 7, 2006, 11:06
Default Hi, Thankyou for your respons
  #4
Member
 
Ivor Clifford
Join Date: Mar 2009
Location: Switzerland
Posts: 91
Rep Power: 8
cliffoi is on a distinguished road
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)
cliffoi is offline   Reply With Quote

Old   November 7, 2006, 11:15
Default Thanks Hrv Seeing the equatio
  #5
Member
 
Ivor Clifford
Join Date: Mar 2009
Location: Switzerland
Posts: 91
Rep Power: 8
cliffoi is on a distinguished road
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
cliffoi is offline   Reply With Quote

Old   November 7, 2006, 11:31
Default Looking at your scheme, it loo
  #6
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
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
hjasak is offline   Reply With Quote

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

Regards
Ivor
cliffoi is offline   Reply With Quote

Old   November 8, 2006, 07:36
Default You mis-understood me: the ope
  #8
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
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
hjasak is offline   Reply With Quote

Old   November 8, 2006, 09:57
Default Right you are Hrv: I had anoth
  #9
Member
 
Ivor Clifford
Join Date: Mar 2009
Location: Switzerland
Posts: 91
Rep Power: 8
cliffoi is on a distinguished road
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
cliffoi is offline   Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Question about the fvmatrix and Laplacian operator liuhuafei OpenFOAM Running, Solving & CFD 6 October 3, 2009 06:58
mixture type material as a phase material Pablo FLUENT 1 January 25, 2007 11:54
laplacian of temperature seyed Farid hosseinizadeh FLUENT 0 December 17, 2006 22:56
Material interfaces using the laplacian operator cliffoi OpenFOAM 0 November 6, 2006 11:42
Laplacian of a scalar value J. Park FLUENT 0 September 17, 2003 12:39


All times are GMT -4. The time now is 06:30.