No drills in slot layers


#1

Hi all,

I’m a new bee in Kicad, as my background is mostly mechanical or welding, but i really like open source projects, linux, debian, freecad or Salome …

My question:

  • i draw some schematic for a car battery charger - SLA 12 V cell -

  • then footprints, linked them with schematics, pcb board, up to now everything is ok

  • exported with Fab files, but can’t see holes and slots in pdf files!!!

My board manufacturer sent me the same error message.

Is there an option or something, i’ve forgotten to follow?

I planed to use an hyperlink to this board, but can’t as a new user,it seems.

                                       Thanks a lot.

                                    jm

#2

You can post a screenshot as a new user. (One image per post. Be careful there is a maximum number of posts per day for new users.)

So please provide a screenshot of the affected area from within pcb_new and one of the resulting pdf. (Maybe add some annotations to it if necessary.)

When you create a screenshot, make sure no personal information can be seen on it.
To post it simply drag and drop it into the answer field.

Also provide us with your kicad version.

What where the steps you made for exporting your pdf? (Did you use plot or print dialog? What are the settings of this dialog?)


#3

Hi Rene and kicad forum,

First thanks a lot for your quick reply.

Kicad version: 4.04 + dsfg1-stable release build

For short, as i can only post one screenshot on forum, i prefer using email:

  • on CAM350 V 9.5.1 plot Separate Sheet from board manufacturer, no hole no slot !!!

  • an other error message from the same manufacturer : see Drill-Map-No-Hole-No-Slot

I’m really disppointed because, i use same footprints from a previous board which works, so ???

See Screen-Capture PCB:

Commands i use in Kicad:

  • Print -> Preview I can see holes Print 1-20 -> Print 10-20

  • File -> Plot -> PDF No Hole No Slot!!!

Would you kind enough to tell me, option or detail, i’ve forgotten?

                                                          Thanks a lot .

                                                              jm

CAM350 V 9.5.1 _ Plot Separate Sheet - -Untitled-.pdf (97.4 KB)


#4

Hi all,

Kicad version: Kicad4.04 dfsg1-stable release build

I misunderstood manufacturer reply…

In fact - see capture screen joined - slots are not found by manufacturing firm.

Is there anyone who can tell me, how to correct this?

Thanks a lot.

                               Jean-Michel


#5

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.)


#6

Hi René,

Thanks for your quick reply, and happy new year for you, your family and members of this forum and users of Kicad.

I sent from earlier, gerber from plot command, not print.

I tried many things:

  • set parameters of 4 holes - see screen capture of drl map .gbr to all pads of the pcb: not good idea as same result as previous…

  • thought about pieces of previous cuts remaining, not one found.

Now, i’m really disappointed as i have tried many, really many trials on this pcb.

Joined steps to get gerber files.

Step 1:

Step 2:

Step3:

                                              Thanks a lot.

                                               Jean-Michel


#7

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)


#8

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.


#9

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.

  1. 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 :slight_smile:
  2. user upgrades to newer version of KiCad, but doesn’t change footprints. New KiCad now outputs G85 for oval holes, fab and user unhappy :disappointed:
  3. 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.


#10

Thanks Bobc,

I’m going to ask pcbway, the way - ok not a good sentence ::::::((((((((((( - how they manage slots.

I’m also going to check on what layer, i draw the outilne… Maybe a mistake on this side.

                      Happy new year.

                            Jean-Michel

#11

René,

Thanks a lot again.

You are not blind, be reassured.

Really, i made a mistake, in first pcb .

Pad properties of SCR and BCxxx oval, and same length for x and y.

Then i change properties to oval, with different lengths for x and y. Make sense, i hope!!! See last pcb draft.png.

See close view or SCR and BCxxx joined.

Pad properties too.

I’m going to ask pcbway, how they manufacture oval holes also.

Maybe triying release 4.07 also.

                             Jean-Michel


#12

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)


#13

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.)


#14

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.

  1. 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.

  1. 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.

  1. 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.

Going to 4.0.7.


#15

Make sure you change the drill type to round, setting x=y with oval will probably not work.


#16

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.


#17

Thanks René,

I’ve just finished this pcb, and everything seems ok, with drl map.

See screen capture joined.

Your advices are really helpful.

               Great, i like opensource and forums like this.

                                             Jean-Michel


#18

Hi Bobc,

You are perfectly right…

I confirm that setting x=y with oval, doesn’t work

As i said to René, i’ve just finished this pcb, and it seems ok for now.

See picture joined.

Many thanks for your advices.

                          Jean-Michel


#19

Hi Hermit,

Thanks for your help and advice.

I’ve just finished this pcb, and it seems ok for now.

See picture joined.

                                Jean-Michel