Rectangular Through Hole Pad Setup

I have a GLCD module with some odd rectangular tabs that are used to connect the LED backlights. I’ve created them to the correct size and location, but they don’t seem to connect correctly to the board. The ground pin will not connect to the ground plane automatically and it looks like the pad is covered by soldermask so I can’t be soldered in the 3d view.

Also, I really only need to be able to solder the part from the opposite side that the part is mounted on.

I can’t seem to figure it out, but I’m sure it’s simple.


attach the footprint you got and a link to the datasheet of the part for that footprint (should contain the fp drawing)


CFAX12864T1-TFH_128x64_GLCD_SPI.kicad_mod (1.5 KB) (389.3 KB)

Are you having trouble with pad/pin 1&2 or the mechanical tabs (that have no number)?

I also can’t figure out how the backlight drawing relates to the other drawings in that datasheet… it seems way too small?

Anyhow, the pad 1 is missing the B.Mask.
Both pads don’t need F.Silk or B.Silk.

If you changed these things in the fp editor and it won’t ‘appear’ in the pcb layout/3d do the following:

  • right click on the display part/footprint in pcbnew
  • select ‘Edit Parameters’
  • click on ‘Change Footprint’
  • change options how you see fit and click on ‘Apply’
    (if you saved the ‘new’ footprint in another library or under a different name you have to go with the List Footprints button)

Yea, it’s a crappy drawing and doesn’t provide any specific footprint dimensions. I derived them as best I could.

I still cannot get the pads to work correctly. They just seem to give me a plated through hole and no pad.

The square cutout for the mounting tab seems ok, but the through-hole pad it not right.

I hope you take the measurements off a real specimen and not just from those drawings… would be a shame to have pcbs made that don’t fit that thing.

Try this one:

CFAX12864T1-TFH_128x64_GLCD_SPI_JTS.kicad_mod (2.8 KB)

I modified the pads and holes a bit.
Also Courtyard needs to be a little bit larger than the actual device… it gives you ‘breathing space’ for assembly.
The device outline is being drawn on Fabrication layer.

Also make sure the edges of those long holes/slots for the retaining hooks has the correct dimension on the inside, otherwise your LCD won’t hold onto the pcb.
The drawing says the retainers are 16.9 mm from inside to inside and the outside is 19.0 mm. Thus they would need to be 1.05 mm from the outer dimension of the housing if that translates directly… that’s where I put them. But if you have a real specimen you can make this better.

@gismofx There may be any issues on that version of 3d-viewer to render that hole type.
Trust only the gerber viewers and what you send to pcb manufacturer.
On that case I also recommend if you can use an oval shape pad.

I think I got it to work correctly. I verified the dimensions of the display with calipers, it’s actually a pretty accurate drawing, albeit odd.

I’m now trying to work around OSHPark’s plated slot hack…This seems to mess up the rats nest and DRC when putting a slot on the edge cuts layer with a pad right on top of it.

Has anyone successfully created a plated slot with OSHpark? Any tips?

Did you try sending them a file from the footprint Joan_Sparky gave above ?
Surely most PCB houses these days can simply read slots in excellon ? No hack needed…

Real slots have radius ends, so it makes sense to see them as such. If you have to fit a metal rectangle inside that, you need to adjust the slot slightly to allow for the radius ends.

Checking the Excellon data of KiCad Slots shows them tagged with G85,G05 and they seem to import fine into GerbView.