9
\$\begingroup\$

Is it okay to connect the exposed pad to the ground pins as in the image below, or is there a recommended way to do it?enter image description here

\$\endgroup\$
  • \$\begingroup\$ It's fine, but see my answer to your other question. \$\endgroup\$ – The Photon Jan 20 '13 at 18:25
7
\$\begingroup\$

One of the most important functions of an exposed pad is heat dissipation. Good heat dissipation requires a strong connection to the ground plane.

If you're dissipating a lot of heat, this often means placing some vias within the pad. These vias must be tented (How do I define a tented via-in-pad in Eagle?) or solder will flow through the via during reflow. Check out SMSC AN18.15: PCB Design Guidelines for QFN and DQFN Packages for details on via placement and solder paste distribution for via-in-pad design. The downside to this approach is that your PCB will cost slightly more to fabricate because of the via-in-pad.

A second option is to use a topside ground pour to heatsink the chip. Connect the center pad to the ground pour through the outer ground pins and place vias in the topside ground pour to your main ground plane. See Micrel Application Hint 17: Designing P.C. Board Heat Sinks for the math on how big of a ground pour you would need. Be careful to connect enough copper to the right side of the chip for proper thermal relief or you may have soldering issues (see Eagle Quicktips: Thermal Relief).

If the chip in question isn't going to be generating significant heat, what you have right now is fine. Just make sure that the return path to your ground plane is as short as possible.

\$\endgroup\$
  • \$\begingroup\$ Sorry to comment on such an old post, but can you clarify if vias within the exposed pad "must be" or should be tented? I'm using a software that does not allow tented vias, but I'd like to get a good connected from the EP to my inner ground plane. Is it the worst thing in the world to have solder get in the via? \$\endgroup\$ – dpwilson Nov 16 '15 at 14:05
  • \$\begingroup\$ The reason they should be tented is that the solder will wick into the via holes and away from the thermal pad on the chip, which may not leave enough solder for a good connection. If you plan on hand-soldering with a hot air gun and will check each chip to make sure it's in place, that shouldn't be a problem, but if you're doing bulk reflow soldering there's a chance some of the chips won't get properly soldered to the board. You'll need to find a balance: enough solder to fill the vias and secure the chip, vs so much solder that it floats the chip too high for the pins to make contact. \$\endgroup\$ – download Nov 17 '17 at 19:32
0
\$\begingroup\$

You might want to add some copper where the trace hits the ground fill - I tend to dislike 90 degree angles in PCBs. In fact I tend to prefer large fills for this purpose. I would even go so far as to completely fill in the area between the two pins shorted to ground. However this will make soldering the component somewhat more difficult due to the heat being drawn away from the pads, so it's your call. I would at least remove the 90 degree angles connecting the fill to pads and just pretty up the top one in general with some 45 degree angles, not whatever random angle that is. Just for looks.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.