I need to place 1.27mm through hole Pin Headers (SWD/JTAG) on my pcb. In KiCad the associated footprint has an annular ring size of: 0.175mm.
The Aisler PCB Design Rules in turn tells me to use a min. annular ring size of 200 μm (0.2mm).
Does this really mean aisler can’t make PCBs for 1.27mm through hole pin headers? Is there any workaround? For example increasing the annular ring for the specific 1.27 pin header footprint?
Thanks for help
Plated holes are compensated with 150µm for manufacturing on our side. This means your 0.65 drill will get compensated to 0.8mm and the annular ring will go to 100µm.
Uncompensated Footprint & Drill = 1mm pad - 0.65mm = 0.35mm / 2 = 175µm annular ring
Uncompensated Footprint and compensated Drill = 1mm - 0.8mm = 0.2mm / 2 = 100µm annular ring
If you increase the Pad size to 1.1mm we will get 1.1mm - 0.8mm = 0.3mm / 2 = 150µm annular ring.
The smallest annular ring we support AFTER compensation is 125µm. So you can increase the pads by 100µm and it will work.