How can I fill the complete pad with polygon pour ? (I dont know the correct question in english)

I am using Altium Designer 17

enter image description here

  • 1
    \$\begingroup\$ Most likely you want to set the polygon pour to not have "thermal relief". There are times this is justified, but beware it complicates soldering! \$\endgroup\$ Oct 8, 2019 at 14:03
  • \$\begingroup\$ will be only for one pad \$\endgroup\$
    – asterix
    Oct 8, 2019 at 17:46

1 Answer 1


Couple of ways to do this either on an as-needed basis or globally. On every design I create a rule as seen in the photo. Then, for example, if you want just a select number of pads (on a net that I may not want ALL pads flooded for that net) flooded with copper I will create a small polygon (to place on top of the parent polygon) just big enough to cover the pad in question and name this polygon "Pin Flood".enter image description here

Or, if you want ALL pads flooded for ALL nets then just change the default "PolygonConnect" to Connect Style==>Direct Connect.

And for lesson #2. You can also create a Pad Class as you see in this photo. enter image description here

Then create a new rule in Polygon Connect that you see in this photo. enter image description here This method is a bit more portable and easier to manage.

EDIT ...and as Chris Stratton points outs above. Flooded copper on TH pads may complicate soldering in terms of proper wetting of the solder fillet. One can always change the rule set from "Direct Connect" to "Relief Connect" and fatten-up the thermal ties.

  • \$\begingroup\$ Ooooh great!! Thanks I need only for terminal screw power supply \$\endgroup\$
    – asterix
    Oct 7, 2019 at 23:24

Your Answer

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

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