Detected Unsupported Drilled Slots (oshpark)


Highlighted in blue in the attached picture is a warning that OshPark Gives me when uploading my gerbers. Does anyone know what the problem may be?
I tried reading this page:
however I don’t understand what is wrong with my project. Does anyone know? It would help me greatly.


The problem is that you have a non-circular hole somewhere on your board. The page you linked gives all the details. Without seeing your project, it’s hard to say more. You could post your project if you want someone here to try to help.

Or, just contact OSH Park support. I’ve found them to be very helpful.


Or just the footprint that has the slot


Thank you all so much for your great answers!
This is my project PCBNew, and GerberView. If the problem is non circular holes as you say it is, then it must be the micro USB port on the top left of the board. I attached the datasheet for that as well.


Make a screenshot of the pad settings of these oval pads.
(or simply upload the footprint here)

It looks like the annular ring for them is quite low. Might be a good idea to increase it.


I assume this is what you guys meant by “footprint”

This is the footprint file code:

(module Connectors:USB_Micro-B (layer F.Cu) (tedit 5AF3C896)
(descr “Micro USB Type B Receptacle”)
(tags “USB USB_B USB_micro USB_OTG”)
(attr smd)
(fp_text reference M-USB (at -0.32592 -4.61602) (layer F.SilkS)
(effects (font (size 2 2) (thickness 0.15)))
(fp_text value USB_OTG (at 0 5.01) (layer F.Fab)
(effects (font (size 1 1) (thickness 0.15)))
(fp_line (start -4.6 -2.59) (end 4.6 -2.59) (layer F.CrtYd) (width 0.05))
(fp_line (start 4.6 -2.59) (end 4.6 4.26) (layer F.CrtYd) (width 0.05))
(fp_line (start 4.6 4.26) (end -4.6 4.26) (layer F.CrtYd) (width 0.05))
(fp_line (start -4.6 4.26) (end -4.6 -2.59) (layer F.CrtYd) (width 0.05))
(fp_line (start -4.35 4.03) (end 4.35 4.03) (layer F.SilkS) (width 0.12))
(fp_line (start -4.35 -2.38) (end 4.35 -2.38) (layer F.SilkS) (width 0.12))
(fp_line (start 4.35 -2.38) (end 4.35 4.03) (layer F.SilkS) (width 0.12))
(fp_line (start 4.35 2.8) (end -4.35 2.8) (layer F.SilkS) (width 0.12))
(fp_line (start -4.35 4.03) (end -4.35 -2.38) (layer F.SilkS) (width 0.12))
(pad 1 smd rect (at -1.3 -1.35 90) (size 1.35 0.4) (layers F.Cu F.Paste F.Mask))
(pad 2 smd rect (at -0.65 -1.35 90) (size 1.35 0.4) (layers F.Cu F.Paste F.Mask))
(pad 3 smd rect (at 0 -1.35 90) (size 1.35 0.4) (layers F.Cu F.Paste F.Mask))
(pad 4 smd rect (at 0.65 -1.35 90) (size 1.35 0.4) (layers F.Cu F.Paste F.Mask))
(pad 5 smd rect (at 1.3 -1.35 90) (size 1.35 0.4) (layers F.Cu F.Paste F.Mask))
(pad 6 thru_hole oval (at -2.5 -1.35 90) (size 0.95 1.25) (drill oval 0.55 0.85) (layers *.Cu *.Mask))
(pad 6 thru_hole oval (at 2.5 -1.35 90) (size 0.95 1.25) (drill oval 0.55 0.85) (layers *.Cu *.Mask))
(pad 6 thru_hole oval (at -3.5 1.35 90) (size 1.55 1) (drill oval 1.15 0.5) (layers *.Cu *.Mask))
(pad 6 thru_hole oval (at 3.5 1.35 90) (size 1.55 1) (drill oval 1.15 0.5) (layers *.Cu *.Mask))


I would recommend just changing the holes in that footprint so that they are circular. (Use the larger of the two dimensions of the oval.) It will require a little more solder to fill the hole, but it will still work fine.


I thought OSHPARK was ok with slots… digging finds

and that says
Slots with unsupported specs Slots width a width less than 40 mil

Looks like you have gone too fine in the slots (tho it wold help if their message said that !)
Given the holes
(pad 6 thru_hole oval (at 2.5 -1.35 90) (size 0.95 1.25) (drill oval 0.55 0.85) (layers *.Cu *.Mask))
(pad 6 thru_hole oval (at -3.5 1.35 90) (size 1.55 1) (drill oval 1.15 0.5) (layers *.Cu *.Mask))

the smaller one can become a hole and the larger one you could try a 40 mil oval ?

I would also increase the annular ring significantly, so you have more solder grip area.


Not only for solder grip but also to have more allowance for milling tolerances.


As an alternative you could use a 100% SMD USB connector.
These usually also have mechanical pads, and if you use a few vias in each of those pad’s they are also fairly strong.


The footprint actually comes with KiCad.

1: How do I change the size?
2: I am concerned with my footprint being permanently changed. Is there a way to do it with the change applying just to this very specific project?



I chose through hole just because it would be easier to hand solder :wink:


I’d just give it a slightly different name after the change.

I know there is the option of saving Symbols and Footprints in each individual Project, but I can’t wrap my mind around exactly why this makes sense if you keep your own local Global library (like I do).

But, if you don’t have your own Global library, then you should make those items available to the Local Project because future changes in the KiCad library may break your design.

If I find a problem with something, I want to fix it across all of my current designs. I don’t want to have to fix the same item five different times, or move and export, whichever makes more sense.


it would be nice to have an ‘annular’ checker implemented directly in KiCAD


just as a workaround you can use


On my linux box at least all the standard libraries are read-only.
No way of accidentally changing them.
But if you want to be sure, make an explicit copy of the footprint and edit that.
It is also always good practice to:
PCBnew -> File -> Archive Footprints ->
and then make an archive lib for each project, or “create library and archive footprints”.
Making such a copy should insure the integrity of your project if the “official” libraries change.


I had one part which had an oval drill but both the diameters were the same, essentially making it a circle. However, OSHPark still saw that as a slot. If is a circle, then just select circle in the footprint’s drill option.


Yea I changed them into circles. Thank you.


This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.