I’m trying to build a footprint for a 0.05" pitch edge connector so that I can either surface-mount or alternatively use pin-headers. A bit like the one I’ve put below (sorry, single image as I’ve only just registered to post)
I thought I’d cracked it with a rounded rectangle shape with offset-hole but then a mate checking before I sent the board off pointed out I’d got the SMT pad on the bottom copper layer as well as the top. I only need the hole and surround on B.Cu not the whole pad that’s on F.Cu.
Editor | Top view | Bottom view
As you can see, I’ve managed to get what I want with pin 1, by using a surface mount pad with an embedded through plated hole. But (I think) this means the schematic needs each pad defining separately? Which is not ideal as it complicates things rather unnecessarily.
I’ve almost managed to get pin 2 to do what I want by using only the F.Cu, and retaining the hole, but it’s (obviously) got no copper on the bottom and possibly not any through.
Pin 3 is the original method of a pad with hole on both copper layers.
Is there an obvious way to do this that I’m missing? Should I start with a hole and extend it rather than starting with a pad and piercing it?
I’d create SMD pad, and put a TH pad with same number over the SMD one.
The method used for pin 1 is the way to go.
No. Just make sure that both the hole and SMD pad have the same pin number and they will get connected to the same schematic pin.
Edit: whoops, should have read the replies too …
Ah, that’s what I tried to begin with, but it gave me a load of DRC ‘Pad too close to pad’ errors. Seems to be fine now, I think I was getting in a mess with library footprints versus that on my board. Spelling it out has pointed me in the right direction. Thanks.
Are you trying to create castelated holes
No @Naib. Just plain holes. The ones one the daughter board aren’t even castellated. But thanks. I was down the right track but wasn’t updating my footprint on the actual board properly.
No, you do not need to assign separate pins for assembly and through-hole pads in the schematic. You can add multiple pads to the footprint. Just assign the same pin number for all the pads. It will be considered as a single pin with the same net names.
For a through-hole pin, having a 50mil pitch is significantly less. Pin headers normally have 40 mils as drill size. So, if you are considering 40mils as drill diameter, then the pad should be around 64mils. Confirm the minimum hole size as per the lead size of the header since it requires at least 8mil clearance between two pads.
I have taken a footprint with five pins, namely, pin 1, pin 2, pin 3, pin 4, and pin 5.
Actually, it has 10 pins; five for assembly and five for through-holes. But here, I have assigned the pin number to assembly pads only. Through-holes will be overlapped.
Front copper for assembly pads:
Bottom copper for through-hole pads:
Top and bottom copper for assembly and through-hole pads:
I don’t know what exactly went wrong and where, but using multiple pads with the same pad number is very common and normal practice in KiCad. It is for example used in lots of footprints in the default libraries. Just search for “thermal relief” in the footprint libraries.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.