Custom Through-hole Pad Polygon Shape

[bradyte]

Hello!

I’m trying to make a custom footprint for the 59S1AC-40MT5-Z SMT Fakra connector. The PCB footprint drawing document shows a unique landing pattern for handling robust mounting.

The connector is SMT but the grounding mounting “nubs” sit in the through holes with solder filling them on both sides.

The footprint shows a rounded pentagon of exposed copper. I’ve made the footprint using the through pads but now trying to impose the additional layout requirements. The issue I’m trying to overcome is not having the thermal relief on the exposed copper and then also trying to combine the through hole pad copper with the exposed copper.

Here is a screenshot of where I’m at on the bottom but I would like the through-hole pad example on the top.

I feel like I’m missing a simple setting but any guidance is welcome.

[scandey]

When you edit a footprint, you can add polygons in any shape you like and combine those shapes with through hole pads. The way I would go about making one quarter of this footprint is:

• Place through hole pad
  
  
• Draw polygon from pad
  
  
• Select the through hole pad and press Cmd+E to enter Pad Edit mode
  
  
• Immediately press Cmd+E again to exit Pad Edit mode
  
  

End result:

[paulvdh]

KiCad has a quite nice system for the thermal reliefs. Normally you set the thermal relief parameters in the zone properties, but this can be overridden either in the footprint (for the whole footprint) or in the pad properties of individual pads. The setting is in: Pad Properties on the Connections tab page.

[bradyte]

Worked like a charm, thank you! Knowing this I will fix some other symbols I’ve kludged!