What exactly did you sent to your manufacturer? (From your earlier posts i would guess you send some pdfs. This is a bit non standard. Normally one would use the gerber format for communicating with manufacturers.)
It might just be that the software your manufacturer uses does not understand the gerber commands for oval holes. Talk to them how they want them to be communicated. (Some like a cutout on edge cuts, some like overlapping drills, some don’t offer oval “drilling” at all.)
I also can’t see the oval holes in the screenshot of your first post. (Either i am blind or there is something wrong with either your kicad version or your footprint) Could you show a screenshot of the pad properties?
Maybe try updating to the current stable release (4.0.7)
It’s difficult to give standardized advice on slots, because it depends on manufacturers and their capabilities. According to the Excellon spec, G85 Drill Drag can be used to specify slots, but it depends on CAM software to interpret that as a milling instruction, not a drill. There are also Excellon commands for milling. These commands may not be supported by all CAM software, you need to ask the manufacturer.
CAN 350 v9.5.1 is an old package (circa 2007) but nevertheless still widely used (upgrading is expensive). If the software doesn’t support slots, then the CAM operator must add them manually. How that is communicated depends on the manufacturer. Some are open and informative eg. http://docs.oshpark.com/troubleshooting/cutouts-and-slots/ otherwise you need to ask them.
If you have instructions from the manufacturer on how to specify slots, then we can advise how to achieve that with KiCad. Usually it just a simple case of drawing lines on a layer such as ECO1.
Ok, I think I have figured what is going on… the OP is not trying to create slots…the fab is telling him he has invalid slots.
a design is created using an older version of KiCad. That version has footprints that have oval holes. Since you can’t drill an oval hole, KiCad simply output a drill instruction to the Gerber. Gerbers are sent to the fab, fab and user are happy
user upgrades to newer version of KiCad, but doesn’t change footprints. New KiCad now outputs G85 for oval holes, fab and user unhappy
KiCad Librarians realise that oval holes in footprints are causing problems, and change all holes to circular.
The way to fix this is to update all your footprints which use oval holes to use circular holes. You can either create your own versions of footprints (less disruption to current PCB), or download a more up to date set of footprints, but that can cause other problems.
I would fix up your current PCB, but I recommend starting any new designs with KiCad 4.0.7 and the footprints that came with it.
Some parts like usb connectors require oval holes (or very large circular holes. This might not be possible for all parts.)
Currently the KLC does not state that oval holes are not allowed. (It does not even require an alternative without oval holes.)
I think a lot of such footprints within the lib have a second footprint that does not use oval holes. But definitely not all of them.
I created an issue over at the repo for this discussion: https://github.com/KiCad/kicad-footprints/issues/214
Do you know what the difference in oval pad handling is between pre version 4 and version 4 gerber output? (If i read your first two scenarios correctly, both use some sort of gerber instruction(s) to tell the fab that there should be an oval hole.)
Maybe a “fallback” mode could be added to convert oval drills back to the pre version 4 format. (If that format has a larger chance of being supported by fabs)
From your screenshots it does not seem that you really require oval holes. If the fab offers them i would guess that it might cost extra. (It is an additional tooling step.) So it might really be better to convert your holes to circular holes. (In this case)
0.8mm is not that much larger than 0.6mm and from the screenshot it seems you have enough copper left to use a circular 0.8mm hole. (make sure you respect both manufacturing and part tolerances when choosing drill sizes. Also ensure that the annular ring requirements of your fab are not violated if you change it to be a circular drill.)
The OP is not trying to create slots , the fab is telling him he has invalid slots: bingo, you 're right, i don’t need slots, not panellised pcbs by exemple.
a design is created using an older version of KiCad. That version has footprints that have oval holes. Since you can’t drill an oval hole, KiCad simply output a drill instruction to the Gerber. Gerbers are sent to the fab, fab and user are happy
Yes, i use an old version of kicad, 4.0.4, but first i set pad properties for SCR and BCxxx to oval, and same length for x and y.
Changed lenghts o different values, after.
Result: Slot missing said by manufacturer board.
user upgrades to newer version of KiCad, but doesn’t change footprints. New KiCad now outputs G85 for oval holes, fab and user unhappy
I’m still unhappy - bad beginning of this year ::::::::::::::::::::)))))))))))))) - but not upgrade to newer version.
KiCad Librarians realise that oval holes in footprints are causing problems, and change all holes to circular.
So, i’m going to change oval to round and same x and y lenght, for footprints and pad properties too.
I ran into this with a barrel jack. I noticed when checking the gerbers the holes were wrong. With the nightly if I chose “Gerber X2(experimental)” printing the drill file the gerber would print out OK. I had a mistake on that board and never fixed it and got it made though so I don’t know if the manufacturer would have accepted it.
