I designed an SMT footprint for a pressure sensor, just 4 SMT pads. The sensor has 2 small protrusions on the bottom used to locate the part on the board for assembly. I could accomodate the protrusions by adding 2 thru-hole (TH) pads to my footprint, but it seems I don’t have access to TH pads while working in a SMT footprint.
I’ve searched around and I see some people have overlayed a via or something else with a hole in it, but then there were DRC errors detected and called out which was kinda messy.
Can anyone point me toward a solution?
Thanks very much!
Hi and Welcome to the forum !
firstly select your project and then hit ‘Footprint Editor’ then scroll down the left hand side and select your library and select the footprint to be worked on from here at the top you will see an option called ‘Place’ and select it then right at the top select ‘Pad’ this will and a pad to the working area. From here you will hover over the ‘Pad’ and hit the ‘E’ key for edit and 'Pad Properties page will appear. From this point it will become clear so at the top ‘Pad properties’ select NPTH Mechanical don’t worry about X Y positions just yet, set shape to circular and diameter to 0.1mm. Below that hole shape is circular and whatever the dimension is for the device locator a common one is 1.2mm. Hit ok and it will appear by your device. Now you need to find the correct position for the holes from the datasheet when done save your footprint. I hope this sorts it out and I just ran through the process in 7.0.2 and it worked fine
@mousey: Thank you for the detailed description! My only concern here is that I want to avoid non-plated holes as they add to the PCB cost. I would be happy with a via or just slapping on a thru-hole pad, but I’m not seeing a way to do that. Thanks again!
. I would be happy with a via or just slapping on a thru-hole pad, but I’m not seeing a way to do that
For a better seeing you have to purchase new glasses.
For the THT pad there as also a solution:
on adding a new pad kicad decides on the footprint-type which pad-type it adds:
for a SMD-type-footprint: every new added pad is always a SMD-pad (as this is the normally needed pad-type)
for a THT-type-footprint: every new added pad is always a THT-pad (same reasoning)
so add a normal SMD-pad to your SMD-footprint
than doubleclick these pad → pad properties dialog opens
now change pad to THT-pad
adjust all other pad-properties (especially pad-diameter / hole-diameter / affected layers)
via inside a footprint is not possible, you have to use the THT-pad)
It could be that you get a “false pad for this footprint type”-warning (or similar) later on the DRC-check, but you have to check (and possibly accept) this. There was some change regarding this check in the past, I don’t know the actual state of this check.
Thank you @mf_ibfeew !!
You are right, of course. I went to see my optomitrist, who issued me a new pair of glasses. I then noticed on the horizontal icon bar the icon “edit the pad properties used when creating new pads”. Using this function allowed me to add 2 new circular thru-hole pads. So now I have a footprint with mixed pad types: 4 pads in SMT and 2 pads in TH. Perfect!!
I am very new to Kicad, coming from PADS Power PCB. All PCB programs do the same thing, but they do them quite differently. With help from users like you in the Kicad community I am finding my way in Kicad. Thank you!!
Hi ! just a quick point, I use JLCPCB to get my boards made and it dosent cost anymore to drill a plain hole and I use a lot of components that have locating pins and never had to think about it so I’m not sure you need to worry about cost, just a thought
