CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   Heat sink analysis (

Scott Hansen October 27, 2008 23:59

Heat sink analysis
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!

Glenn Horrocks October 28, 2008 00:34

Re: Heat sink analysis

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

Scott Hansen October 28, 2008 01:05

Re: Heat sink analysis
Thank you very much, do you happen to know where I can activate the option to automatically generate GGI interfaces? Thanks

pratik mehta October 29, 2008 07:00

Re: Heat sink analysis
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

Glenn Horrocks October 29, 2008 21:28

Re: Heat sink analysis

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

MarkoP May 6, 2015 05:52

1 Attachment(s)

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?


You can see here what it looks like...

Attachment 39256

singer1812 May 6, 2015 09:10

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.

MarkoP May 6, 2015 10:19

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!

singer1812 May 6, 2015 10:32

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).

All times are GMT -4. The time now is 10:50.