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

Heat sink analysis

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 27, 2008, 23:59
Default Heat sink analysis
  #1
Scott Hansen
Guest
 
Posts: n/a
I am trying to use CFX to model the performance of a heat sink that I am designing as part of my mechanical engineering senior design project. The way I have I have it set up is there are 3 regions:

1.) Electronic chip, modeled as a small rectangular prism. It generates 13W of heat.

2.) The actual finned heat sink, modeled originally in Pro/E.

3.) The air domain, which surrounds the heatsink and is box-shaped on the outside.

My problem is that when I mesh all these together in Ansys (using different element types, of course, for the solid and fluid regions), CFX does not recognize any distinct regions in the mesh, so basically I just have box. When I don't glue the volumes together in Ansys and import the meshes separately it does recognize the distinct regions, however I don't believe the regions can "talk/interface" properly since they aren't technically connected in any way, just adjacent to each other. Also, I don't get very reasonable results from the solution. Does anyone have any recommendations on how I should set this up? Obviously, it will involve conjugate heat transfer, and I have read the heating coil tutorial that came with CFX in the help file. Thank you very much!
  Reply With Quote

Old   October 28, 2008, 00:34
Default Re: Heat sink analysis
  #2
Glenn Horrocks
Guest
 
Posts: n/a
Hi,

You need to set up GGI interfaces to get the heat transfer happening. There is an option in CFX-Pre to automatically generate these when the geometry is loaded.

Alternately you can make the bodies a multi-body part in DesignModeller then the mesh will be contiguous across bodies. In an ideal world you could then use 1to1 interfaces which should be more accurate and computationally efficient but I think in V11 there is a bug where CHT does not work properly with 1to1 interfaces, to work around this you have to define them as GGI interfaces.

Glenn Horrocks
  Reply With Quote

Old   October 28, 2008, 01:05
Default Re: Heat sink analysis
  #3
Scott Hansen
Guest
 
Posts: n/a
Thank you very much, do you happen to know where I can activate the option to automatically generate GGI interfaces? Thanks
  Reply With Quote

Old   October 29, 2008, 07:00
Default Re: Heat sink analysis
  #4
pratik mehta
Guest
 
Posts: n/a
DO you have problems with ICEM or CFX Pre . If you are experiencing the problem in ICEM during meshing then all you need is to define fluid zones for all the regions

I hope this helps
  Reply With Quote

Old   October 29, 2008, 21:28
Default Re: Heat sink analysis
  #5
Glenn Horrocks
Guest
 
Posts: n/a
Hi,

In CFX-Pre the default interface option is automatic (it will be somewhere in the page with the settings for the interface). Flick it over to GGI.

Glenn Horrocks
  Reply With Quote

Old   May 6, 2015, 05:52
Default
  #6
New Member
 
Join Date: Mar 2015
Posts: 14
Rep Power: 2
MarkoP is on a distinguished road
Hello,

I as well am trying to simulate the performance of a heatsink. I have a heatsink attached to a PCB with some capacitors behind. The whole system is in a duct of air and as BC I have an outlet with normal speed because we'd like to suck the air out and an opening on the other side. Is it normal that the speed at the outlet and the opening are the same and that the pressure at the outlet is bigger than the pressure at the opening which is defined as 0 Pa relative pressure?

Thanks

You can see here what it looks like...

Heatsink Duct.jpg
MarkoP is offline   Reply With Quote

Old   May 6, 2015, 09:10
Default
  #7
Senior Member
 
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 494
Rep Power: 11
singer1812 is on a distinguished road
Increase your domain size. I would suggest adding a lead up and down passage to allow flow to develop as it is in the heat sink domain.

You can get a better pressure drop estimate by doing this.

If your inlet and outlet size are the same, your velocities are going to be the same.
singer1812 is offline   Reply With Quote

Old   May 6, 2015, 10:19
Default
  #8
New Member
 
Join Date: Mar 2015
Posts: 14
Rep Power: 2
MarkoP is on a distinguished road
The duct size is determined already, it should not be changed, I could only do it for purposes of getting a better idea of what happens. For the velocities, they are the same even though there is a whole heat sink, PCB, capacitors inside? I thought they would act as some flow resitance... :?

Thanks a lot btw!
MarkoP is offline   Reply With Quote

Old   May 6, 2015, 10:32
Default
  #9
Senior Member
 
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 494
Rep Power: 11
singer1812 is on a distinguished road
I realize the duct size is fixed (Wxh). I am suggesting adding more leading up and going away from (adjust the leading in L and going away L). Or do you have that in your model and not showing it?

The lead up and away isnt intended to model anything real, it just pulls your imposed BCs away from your "real" domain. I would guess your bcs arent detailed enough to match how the flow is behaving right where you are showing in your pic. Moving them back will lessen the results influence from them. In addition, the pressure loss from a straight section will be negligable to your domain (use free slip walls if you so desire), so you can pull pressures out a little ahead and back from your domain, to remove flow items in how you are retrieving the pressure loss.

If you are fixing inlet flow rate, how do you think the flow will slow down with adding stuff into its path? You are correct, the resistance increases with more stuff, but if you calculate the velocity from inlet and outlet across the same area size, velocities will be the same (conservation of mass).
singer1812 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
Help modeling heat sink aimee FLUENT 1 June 3, 2011 14:17
Simulate heat transfer of heat sink in a box... chien87 CFX 8 February 8, 2011 04:50
Reply me if u did heat sink analysis siva FLUENT 0 January 5, 2009 08:07
Simulation on Heat Sink Ken Adams FLUENT 4 June 26, 2007 16:03
Heat sink analysis Akash FLUENT 2 September 13, 2004 11:14


All times are GMT -4. The time now is 08:06.