1
\$\begingroup\$

Using KiCad, is there a way to have a pad with an slot shape (referred to in KiCad as "oval") be exported properly as a drill (.drl) file? The pad in KiCad looks like Fig. 1 below.

But after exporting the PCB layout to the gerber and drill files, it seems to only process a single round hole, rather than the entire slot/oval, as shown in Fig. 2 (as seen from a separate gerber-viewing program).

I was previously able to work around this problem by modifying the footprint to have multiple smaller circular drills instead of a larger slot/oval one and got it successfully fabricated. Are there more efficient alternatives?

(Fig. 1: pad in Kicad) Pad in KiCad

(Fig. 2: exported pad in gerber viewer) Pad in gerber viewer

\$\endgroup\$
2
  • \$\begingroup\$ That is not an oval, that is a slot. This is apparently a known issue with the G85 g-code command. \$\endgroup\$ – Spehro Pefhany Jul 13 '20 at 2:02
  • 2
    \$\begingroup\$ You will have to negotiate with your board shop as to how it should be documented (or if they could/would do it). They would have to mill the slot, which would probably be a separate operation on a different machine than used for drilling holes. \$\endgroup\$ – Peter Bennett Jul 13 '20 at 2:12
3
\$\begingroup\$

Round holes in the board are made using drill bits in an automatic machine that pokes at the board with a spinny thing,

The DRL file gives the locations and sizes for theses holes. if you make two holes overlap there's a large risk that the drill bit will break so that is against the rules.

slots are made using milling bits in an automatic machine that pokes at the board with a spinny thing and then drags the spinning cutter along a defined path.

2mm is the diameter of the cutter usually used so slots narrower than 2mm, or with corner radiuses less than 1mm may cost extra. Smaller cutterrs are available but because they are more easily broken the cuiting speed is reduced, and because time is money you will pay for that.

PCBWAY asks for the slots to be included on the "Board Outline" Gerber layer, check with your chosen manufacturer on how they want slots presented.

Sometimes you don't need slots, eg CUI makes a 5.5x2.5mm jack with "round" pins, intead of flat tabs.

\$\endgroup\$
2
  • 1
    \$\begingroup\$ "spinny thing" very appropriately named. I like it. \$\endgroup\$ – vini_i Jul 14 '20 at 12:10
  • \$\begingroup\$ Drawing on edge cuts to show this is not really an option in kicad as DRC respects anything on edge cuts and does therefore not allow connecting to a pad that has a drawing on the edge cuts layer. \$\endgroup\$ – Rene Pöschl Jul 14 '20 at 17:19
2
\$\begingroup\$

Drill files only drill round holes. If you want a slot, then design a slot as is explained in one of the Digikey Kicad tutorials on Youtube. You will get a slot.

There's no such thing as a slot that is going to be part of a drill file. Slots are slots and holes are holes.

\$\endgroup\$
2
\$\begingroup\$

Slots and odd-shaped holes are done with a CNC machine, as opposed to just drilling round holes. I was in touch often with the board house about slot cuts, etc. If the drill chart defines a named hole as a oval cut with these x-y dimensions and this milling diameter, then a board house should be able to make them. They do cost more than round holes, and do cost more than in-line slot cuts.

I suggest you contact the board house so they pay close attention to a detailed drill chart. If your layout program cannot do odd-shaped holes then rely on the drill chart and let the program show its default interpretation of the hole. As expensive as these CAD programs can be, their internal library of non-round shapes is very limited. They can do diamond-cuts for RF GND planes but not create non-round holes.

\$\endgroup\$
1
\$\begingroup\$

This might just be a problem with your gerber viewer. KiCad exports the oval holes as a milling path so any fab with modern software should be able to deal with it. I suggest you contact your fab of choice and ask what they make of such a file and what they suggest you use if they can not deal with the way kicad defines ovals.


One thing you might need to know is that one can not simply draw onto the edge cuts layer as others suggested as kicads design rule checker will complain and you then can no longer connect the pad in a normal manner. So if your fab requires such pads to be indicated by a drawing on some layer instead of by use of the special gerber command used by kicad then you might be best off using for example one of the eco layers and tell your manufacturer to use this layer as the source for oval holes. Or you might need to combine gerber layers if the manufacturer really needs the outline and such cutouts on the same layer.


It might also be the case that the manufacturer can in fact deal with the kicad gerber command and only the online gerber viewer has problems with it so maybe just ask their support if they can deal with oval holes defined in the way kicad defines them.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.