CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Setting different conductivity for various regions

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 14, 2018, 04:39
Default Setting different conductivity for various regions
  #1
Senior Member
 
Sasan Ghomi
Join Date: Sep 2012
Location: Denmark
Posts: 206
Rep Power: 9
sasanghomi is on a distinguished road
Dear friends,

I am dealing with a conduction heat transfer problem and I need to specify different conductivity to the regions of my domain. The problem is that I do not want to separate the region into some domains (because the mesh generation becomes difficult). So, my question is that whether or not I can specify different conductivity values for different regions of a specific domain without separating the parts?
For instance, in OpenFOAM by using Cell set utility we can choose specific regions for one domain without cutting the domain.

Is there any solution for this problem?

Any suggestion is appreciated
sasanghomi is offline   Reply With Quote

Old   June 14, 2018, 05:25
Default
  #2
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Posts: 545
Rep Power: 10
Gert-Jan is on a distinguished road
If you don't want to split the geometry into different domains, because the geometry would become too difficult to mesh, then how do you think you can create the regions after the mesh is generated? Selecting individual mesh elements is even more difficult, very laborious and error prone. It sounds very unlogical and I don't see your point here. So, please explain what you want to do.
Gert-Jan is offline   Reply With Quote

Old   June 14, 2018, 18:52
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,057
Rep Power: 115
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
You can define conductivity to be a function of just about anything. So you can make it a function of its location and that way model the variable conductivity without having the region defined in the mesh. But for complex shapes this is difficult and it becomes much easier to just define it as a region in the mesh.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   June 15, 2018, 01:40
Default
  #4
Senior Member
 
Sasan Ghomi
Join Date: Sep 2012
Location: Denmark
Posts: 206
Rep Power: 9
sasanghomi is on a distinguished road
Dear Glenn Horrocks

Thank you so much for your response.
Could you tell me please that how I can set a function for conductivity values (according to position)?

Best Regards
sasanghomi is offline   Reply With Quote

Old   June 15, 2018, 01:48
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,057
Rep Power: 115
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Set the thermal conductivity to:
if(x>10[m],10[W m^-1 K^-1],100[W m^-1 K^-1])

Or use a 1D or 3D interpolation function, or a fortran user function, or one of the many other CEL functions.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   June 15, 2018, 02:24
Default
  #6
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Posts: 545
Rep Power: 10
Gert-Jan is on a distinguished road
You can also use step functions like:


labda = 1[W/m/K]*Step(X)+3[W/m/K]*Step(-X)


giving a value of 3 if x<0 and 1 if x>0 (please check the correct syntax for 'Step' and 'x'. It is just an example out of my head). But if you can use such simple expressions, to describe the conductivity, then why not create separate domains. I still don't get it.



To me this looks like an X-Y-Problem.
Gert-Jan is offline   Reply With Quote

Old   June 17, 2018, 05:19
Default
  #7
Senior Member
 
Sasan Ghomi
Join Date: Sep 2012
Location: Denmark
Posts: 206
Rep Power: 9
sasanghomi is on a distinguished road
I am so thankful for your responses. The problem is that the geometry of my simulation is complicated. It is about winding of an electrical generator. Do you have any ideas that how I can get the function that describes positions of different parts in modelling software programs (Design modeler, Catia, etc.)? Is there any utility?

BR
sasanghomi is offline   Reply With Quote

Old   June 17, 2018, 06:53
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,057
Rep Power: 115
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
For a complex geometry the only way is to define a mesh region as Gert-Jan has been saying all along. Catia and DesginModeller can both do this sort of modification easily, and then you remesh it.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   June 24, 2018, 07:44
Default
  #9
Senior Member
 
Sasan Ghomi
Join Date: Sep 2012
Location: Denmark
Posts: 206
Rep Power: 9
sasanghomi is on a distinguished road
Thank you so much. However, I found a solution that it is possible to consider a thin layer (with specific conductivity) as an insulation in the interface of two parts. So, it is not necessary to create different parts with small thicknesses.

Any Idea?

I appreciate your support.
sasanghomi is offline   Reply With Quote

Old   June 24, 2018, 18:59
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,057
Rep Power: 115
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Yes, that is correct. It is often better to model thin layers as thermal resistance on an interface than to physically model the interface.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks 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
Unkown multiple regions in checkMesh hokhay OpenFOAM Native Meshers: snappyHexMesh and Others 3 August 24, 2017 12:48
Regions setting MechaalAchraf OpenFOAM Meshing & Mesh Conversion 0 June 15, 2017 09:23
Conductivity as a vector value Nurzhan CFX 16 June 5, 2017 10:10
chtMultiRegionSimpleFoam: Thermal Conduction + Surface-To-Surface Radiation Zeppo OpenFOAM Running, Solving & CFD 16 May 18, 2017 18:04
Warning 097- AB Siemens 6 November 15, 2004 04:41


All times are GMT -4. The time now is 01:32.