Jump to content
granzer

How to use thermal shells?

Recommended Posts

I have to model heat conduction and dissipation from a electronic component through a think layer of copper present over a PCB i.e. there is an electronic component fixed to a PCB. Between the electronic component and the PCB there is a thin layer of copper. The copper layer extends beyond the electronic component and can conduct heat form the electronic component and can dissipate it to air. Can I use thermal shells to model the copper layer. If I can then how do I use it? Should I create a separate surface (with out any parent volumes) between the boundary surfaces of PCB and boundary surfaces of the electronic component? 

Share this post


Link to post
Share on other sites

Thermal Shells in AcuSolve can help. Which preprocessor are you using? AcuConsole, HyperMesh, HyperWorks CFDx and SimLab all support thermal shells for the purpose you need. 

 

HyperWorks CFD: Thin  domain

image.png

 

AcuConsole : 

image.png

 

 

HyperMesh: 

image.png

Share this post


Link to post
Share on other sites

I am using hypermesh for meshing the domain and Acuconsole for setting up the case. Should I create a separate surface (with out any parent volumes) between the boundary surfaces of PCB and boundary surfaces of the electronic component? I tried creating 3 surfaces to occupy the same plane but connected at the edges, but one of the surfaces always seems to disappear. 

Share this post


Link to post
Share on other sites

If you are creating the thermal shells within AcuConsole, you'll start with a single set of nodes shared by the PCB and the electronic component.  (There should be two surface definitions - one attached to the PCB volume and the other attached to the component volume - but still using the same set of shared nodes.)  To make sure, you can right-click on each of the volumes, and use Find/Extract Missing Surfaces, in case some definitions didn't carry through from HM.  Once you have both surface definitions, right-click one of the other and create the thermal shells.

Share this post


Link to post
Share on other sites

OK so so creating separate surafaces(one for PCB and one for Electronic component) in HM  OR  if only one one common interface surface was created in HM then 'splitting' the 2 surfaces that gets created in acuconsole for the interface (to have separate nodes for each surface) is not required then? 

It is my understanding that shell elements usually have 2 surface enclosing its o volume, how are they created in acuconsole? I need to understand how the 'default' surfaces created enclose the shell-volume to plot the heat flux going in and out of the volume.   

Share this post


Link to post
Share on other sites

During the 'create thermal shells' process in AcuConsole, the shared nodes on the surface are split, with the 0-thickness volume preserved between them.  I'm not too familiar with the HM process.  In AcuConsole I would typically have the two surfaces defined as mentioned earlier - one attached to each volume, but with the same set of nodes.  (Make sure you have both defined - using the 'Find Missing Surfaces' on the volumes.)  When the thermal shell is created, those surfaces still exist, but updated to the proper nodes.  Then you'll also get a surface set attached to the thermal shells - with both 'sides' in the same set.  You'll still be able to use the surfaces attached to the two main volumes for your post-processing needs.

Share this post


Link to post
Share on other sites

So this is what I understand from "

 Then you'll also get a surface set attached to the thermal shells - with both 'sides' in the same set.  You'll still be able to use the surfaces attached to the two main volumes for your post-processing needs.

"  
i.e. the surface which are created during creation of (and which are attached to) the shell volume are all under a single named surface, say the name of the surface is "default". If that is true then this " with both 'sides' in the same set. " would mean that if I got the value of the heat flux on this 'default' surface it should be zero, as what ever heat is going into the shell volume should be coming out of it to bring the shell volume to a steady state temperature(and the 'default' surface encloses the shell volume from "all"/both sides. But when I do measure the heat flux on the ';default' surface it is not zero. 

Share this post


Link to post
Share on other sites

It looks like I was mistaken.  Based on the area and number of faces in the 'default' shell surface set, that surface set is only one side or the other, not both.  I suppose based on the other two surfaces at that location (one attached to each volume) you can determine which 'side' of the thermal shell that surface represents.  Still better to use the surfaces attached to the original volumes for post-processing.

 

In a case where the edges of the thermal shells are attached to insulated zero-flux surfaces, the sum of the two surfaces attached to the original volumes should be zero (having equal but opposite-sign values).

 

In a case where the thermal shell edges are attached to surfaces that might have heat transfer across them, there could also be conduction in the thermal shell 'cross-direction' so the sum of the other two surfaces may not be zero.

 

 

Share this post


Link to post
Share on other sites

If there are 2 seperate surface,S1 and S2,  attached to 2 different volumes, vol1 and vol2, which are in contact with each other(i.e. the interface between the vol1 and vol2 is made by S1 and S2) and I want to create 2 seperate shell volumes,svol1 and svol2, between these two volumes (ie vol1 and vol2). Can i create svol1 using S1 and svol2 using S2?. Also can I get correct heat transfer between svol1 and svol2?. How will I get the value of heat flux between the two shell volumes ie which surface should I select to measure the heat flux between the 2 shell volumes?

 

PS: I dont want to create just one shell volume and use the layer option.

Share this post


Link to post
Share on other sites

Example can be taken from electronic cooling itself. For example an electronic component might be sitting on a thin square highly conductive plate, and this small plate may itself be resting on a larger thin rectangular plate for heat dissipation. This larger plate is resting on a PCB. So the small square plate and the larger rectangular plate(these two plates would be modeled as 2 separate shell volumes in contact with each other) would be sandwiched between the electronic component volume and the PCB volume.

Share this post


Link to post
Share on other sites

You mentioned you didn't want to use the 'multiple layers' in the thermal shells, but that is exactly the better way to approach this, and the reason for having thermal shells.  You would neglect any potential heat transfer from the edges, and simply assume that anything that enters the thermal shell at one 'end' leaves from the other.  In fact, you could check that by reviewing the heat flux values from the surfaces bounding the thermal shell.

granzer likes this

Share this post


Link to post
Share on other sites

Ok..I was just considering this approach as the 2 shells are different sized squares(say 2*2 and 4*4), but ya since there is no heat transfer form the sides of the shell it has to go form one to the other. Thank you, this has been informative. 

Share this post


Link to post
Share on other sites

×
×
  • Create New...