Laying out footprint with exposed pad


My design has utilizes a battery fuel gauge (LTC2943) which has an exposed pad which gets connected to the ground plane. Is the way I have set pad number 11 correct ? In the layout I will connect pad number 11 to the ground plane. Btw, I will be hand soldering this.


I pulled up a data sheet and it says connecting that pad is optional. Pins 2,3 and 7 are also ground. When you say you are gong to hand solder it do you mean you are going to try and run solder into the holes from the bottom side? Or do you just mean you are going to hand solder the other terminals on the chip? I’m just curious because I have no experience doing what you are proposing and it caught my attention.


Will hand solder all the other terminals. I might change the holes to smd pads and have vias going to the ground plane.

It says it is optional…but I think doing this would help with heat dissipation from the chip.


I haven’t verified dimensions against the datasheet, but it looks basically OK for providing a minimum amount of heatsinking to the IC.

About 2 years ago (when I was just starting with KiCAD) I used Linear’s LTC4011 in a design. It has a similar thermal pad on the bottom of the package, but connecting it to ground is REQUIRED. (A poor, or missing, ground connection causes damage to the IC. Sadly, I know this very well from experience.) On the board, the footprint’s back and front sides look like this (traces omitted for clarity):

These prototypes were intended to be hand-soldered. Note that I extended the thermal pad to create places where it could be touched by soldering irons. Without the thermal pad extensions it is impossible to manually solder the IC.

Even with the extensions, we had 2 or 3 IC failures in the first 5 prototype boards. Then we soldered the IC using TWO soldering irons - one on each end of the IC. That seemed to work if the two irons were very hot. It required two people to do the job, and you had to pay careful attention to avoid burning somebody with a hot iron. We soldered the thermal pad first, to ensure that the thermal pad had good contact with the board. (If you solder the signal pins first, the package body may float up off the board by a few mils.)

I left the vias exposed (no solder mask over the via) on the back side. After soldering we looked at the vias under magnification. If we saw solder filling most of the via holes, or at least partially filling the vias, we assumed that the solder had flowed to that area of the topside pad and made a good joint. If the hole was empty we guessed that there was a void on the topside at that location. I think we decided that two (or three?) unfilled vias (out of 12) was acceptable, but more than that caused us to repeat the soldering process.

Eventually we went to a reflow process, using an electric skillet (from a second-hand store) as a “tabletop reflow oven”. That seemed to give the most consistent results, possibly because everything was heated to the solder’s melting temperature, or close to it.



That’s the way to go.
@MNyasha, enough guides on the internet how to turn any cheap tabletop grill oven (1.5kW+) into a reflow oven and how to apply solderpaste DIY.