4
\$\begingroup\$

I'm making a part in Eagle (4.15) for a SOIC-8 package. There is a thermal pad in the center and I'm trying to add vias stitching the top and bottom pads together. In the Eagle package editor there are no vias, I can add pads or holes. Is there a standard way to do this? I've found some related questions, and this, but no answers that help me.

I'm using an old version of eagle (4.15)

\$\endgroup\$
2
  • \$\begingroup\$ I think the difference between 'vias' and 'pads' is only a matter of terminology and refers to how they are used on the board: either for routing or to solder a thru-hole component. When designing a component footprint there is no difference... \$\endgroup\$
    – brhans
    Mar 30, 2015 at 19:11
  • \$\begingroup\$ @brhans, yeah that's right. My problem is that if I use through hole pads to stick the top and bottom layer together I then end up with a whole bunch of extra pads in my package. I can try leaving these unconnected and see what happens. \$\endgroup\$ Mar 30, 2015 at 19:16

1 Answer 1

7
\$\begingroup\$

Use pads.

You can use an array of pads to create these thermal vias. The difference between pads and vias are that pads always go all the way through, vias can be blind or buried. For thermal vias, you want to go all the way through, so use pads.

If you use holes there will not be an electrical connection through the board, thus minimal thermal conduction. So it's rather pointless and will likely only cause DRC errors related to placing metal (for the thermal pad) too near a drill hole.

Here's an example from my library using pads for thermal vias.

thermal vias

Just connect each of the pads to the same pin as the ground pad. This makes them of the same net before being placed in the layout editor, thus avoiding the pad-to-pad or similar possible DRC errors.

enter image description here

\$\endgroup\$
6
  • \$\begingroup\$ So do you leave all those pads (in the package) unconnected when you connect the package to the symbol? Or do you just make a device with a lot of extra "pins". \$\endgroup\$ Mar 30, 2015 at 19:19
  • \$\begingroup\$ @GeorgeHerold You can add multiple pads to a single pin, just connect all of the pads to the same pin. \$\endgroup\$
    – Samuel
    Mar 30, 2015 at 19:20
  • \$\begingroup\$ Hmm, OK maybe this is because I have an old version of eagle. But in the library editor I can only connect one pin to one pad... unless I'm missing some special key combination. \$\endgroup\$ Mar 30, 2015 at 19:27
  • \$\begingroup\$ Ah, no append button? I checked the release notes for versions 4 through 7 and don't see it being added, so I assumed it was in there. It should be in the connect dialog in the part editor. \$\endgroup\$
    – Samuel
    Mar 30, 2015 at 19:32
  • \$\begingroup\$ Ahh.. what's an append button look like :^) I've just been reading my manual (always a last resort) It says, "One pin has to be connected to exactly one pad!" Their exclamation mark, so I assume I'm stuck in this version. I'll make a bunch of extra pins and stick 'em down with the other power pins.. gotta keep a nice clean schematic. \$\endgroup\$ Mar 30, 2015 at 19:57

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.