Hi Phil,

1) Yes, it is a very common practice
2) Yes, it really provides effective device heat sinking

You didn't say whether you were placing the heat-sinking PTH around the perimeter of the land, or directly in the land area (array). The array is best for high-temp of course, but has soldering challenges. Most people rely on the reflow oven to melt everything at once, and struggle (or give up) on the manual rework. We have people who say they can un-solder ANYTHING, but I cringe thinking about the board damage. One solution that might work is to put the PTHs AROUND the land - let the via pads encroach into the land area, but not the via holes, so the connecting trace length goes to zero, but most of the via is still coated with soldermask to prevent the paste from flowing into the holes (tented vias). Also, in case you didn't think of it, if there is enough open area you can pour extra copper fill around your hot terminations to spread the heat out from the lead. maximize the copper area if it doesn't cause noise immunity/interference issues

regarding the effect of greater board thickness, there are only a few data points related to that in the IPC-2152 document, but until we have anything better, here is IPC-2152 paragraph A.4.2: 

Current carrying capacity testing of conductors in 0.965 mm [0.038 in] thick FR-4 PBs show
results that are 30-40% higher in temperature compared to the 1.79 mm [0.070 in] thick PB
temperatures. The higher temperatures (a 40% increase) are seen in larger conductors (2.54
vs.0.203 mm [0.100 vs. 0.008 in]). Testing with 1.50 mm [0.059 in] thick FR-4 PBs showed
temperatures that are 10-20% higher compared to the 1.79 mm [0.070 in] thick polyimide test
boards.

A little too vague, and take note that they are comparing Polyimide to FR-4 (which is already a 2% difference in paragraph A.4.4), so 
1) use at your own risk, and 
2) encourage all your friends and neighbors to collaborate with IPC to get more data.

Jack (the "cool" guy)


.
On Mon, 19 Dec 2016 18:34:53 +0000, Nutting, Phil <[log in to unmask]> wrote:

>Hi All,
>
>We have several designs in which we use the thru-hole pad and surrounding etch to act as a heat sink for device heat being transmitted via the component leads.  Typically 2 ounce copper and often on 0.090" thick FR-4 boards.  With the added copper thickness and larger pad area for better "heat sinking" we now introduce greater difficulty in getting a quality solder joint and don't get me started on the increased difficulty in removing a bad component.
>
>So my questions are:
>Is this a common practice?
>Does it really provide effective device heat sinking?
>
>Phil Nutting  |  HVP Development Engineer   |  Excelitas Technologies Corp