I am attempting to create a polygon that increases the area of an existing smd pad so as to make the area larger in order to hand solder. I am running into an issue removing what I believe is the thermal boundary between the polygon and the pad.

I read through a couple previous posts with similar issues:

Eagle make copper pour connect to entire smd pad

Removing pad to polygon space in eagle

the pad in question is only there to adhere the part to the board, it serves no other purpose.

I double checked that I was not using thermals when creating the polygon, then modified the footprint and removed thermals from the pad in question as well. Since then I have completely removed and re-added the part to the board, but the issue still persists.

enter image description here

  • \$\begingroup\$ I don't use Eagle but in OrCAD you must assign a net to the polygon. If it matches the net of the pad then it will merge. \$\endgroup\$
    – DKNguyen
    Commented Feb 13, 2020 at 16:11
  • \$\begingroup\$ If you're willing and able to edit the footprint, why didn't you just make the pad larger right there? Create a variant of the original footprint if you want to have both choices available. \$\endgroup\$
    – Dave Tweed
    Commented Feb 13, 2020 at 16:22
  • \$\begingroup\$ One of my initial attempts to solve this issue was changing the pad size, but for some reason I did not like the result. I think in the end I will go back to modifying it. Thanks again for your answer and the comments. \$\endgroup\$
    – Lundy Wyre
    Commented Feb 13, 2020 at 16:48

1 Answer 1


Add a wire to the pin in the schematic named something (like MP1), and just leave it floating. Then in the board view, type ripup @; to view the polygon outline, right click on it and name it MP1 (same as the name of the wire in the schematic). Type ratsnest and you'll see the pour connected to the pad.

BTW, this will connect the pour to the pad, but won't give you a "larger solderable area". The problem is the solder mask will still cover the copper pour. If you want a particular size pad, you need to do this in the part library and not use a copper pour. This will actually make soldering more difficult, because the larger copper area will "wick" away heat from the pad, so you'll have to use a lot more heat to get the solder to melt.

This is why there are "thermals" on pads, they are there to limit the amount of thermal transfer to the copper pour to make soldering easier.

  • \$\begingroup\$ Thanks for the information Dave, your solution worked. At first it was still not connecting, but I realized why. Within the symbol of the library, I did not define a pin to associate to the pad within the footprint. I created a pin (MP1) and connected it to the pad \$\endgroup\$
    – Lundy Wyre
    Commented Feb 13, 2020 at 16:39

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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