I just wanted a nice printout for my own reference and to share online. I’ve ordered the board from OSH Park and they take a kcad_pcb file.
Despite what you say, I do see the holes I expect in F_Mask.pdf and not in F_Cu.pdf.
16buttons-F_Cu.pdf (20.8 KB) 16buttons-F_Mask.pdf (17.5 KB)
Overlay the mask layer over the copper layer. You will notice that the “holes” on the mask layer are way too large for them to represent the drills (check the layers in kicad. You see the mask layer there as well. It will be much more clear to you that this layer is not the thing that defines the drills)
But I don’t see the mounting holes at all in the copper layer. At least in the solder mask layer, I see where they go, even if they’re not the right size.
As mounting holes are non plated, there is no way to see them in copper layer plot.
If you need to see the position of the mounting hole in YOUR plot, place a via in center of mounting hole.
Okay, that makes sense, but I think this is getting off the subject. I just wanted to report that the drill holes (in this case, non-plated mounting holes) don’t show up properly when using “Print”, not “Plot”. I guess there are workarounds.
My workaround (and, it makes most sense to me/my-projects) is to Edit the footprint and change the diameter’s of the Graphic on the Courtyard (Comments and other Layers I want to have more accurately represent the features).
In fact, Different parts have the Graphics on inconsistent layers (e.g. MountingHole has graphic on Comments and Courtyard). I Use Comments exclusively for Comments!!!
Below image shows:
• Original MountingHole/Graphic
• Edited (reduced diameter of graphic on the parts default layer (didn’t bother to change that)
• Screenshot of the Printed board (just used ‘File>Print’)
• 3D View of PCB
Also, I changed the thickness of the Lines (and text) of the Courtyard - screenshot… Shows nice and dark now.
The courtyard layer has a specific reason. It is used for DRC to check that you can mount the part that is connected to the footprint. The fab layer less so but i would still suggest it to have the nominal size of whatever you mount on there.
In the case of a mounting hole i really suggest that the fab layer holds the nominal diameter of the screw head (or whatever is mounted there) and the courtyard layer is slightly larger than the screw head plus whatever tool you need to fasten it.
I think the larger circles on the courtyard and Cmts.User layers are supposed to be about not putting other stuff too close to the drill hole, to leave room for a bolt or nut.
Looking at the MountingHole_2.1mm footprint in the standard library, it seems to represent the drill hole as a pad, showing up on the copper and solder mask layers. Putting it on the copper mask layer doesn’t make sense to me since there is no copper there, but presumably it’s a convention? I also wonder why, if there is copper in the footprint, it doesn’t show up when printed?
… Quick upshot…
I construct work-arounds to meet my needs - I CNC Mill my PCB’s. And, I seldom consider how/what others do/did (been an Engineer for 50yrs!!)
I use the same mountinghole you reference (2.5mm, 3mm and 3.5mm) and there’s no need for me to tweak as I indicated previously.
However, after posting above, I thought about it and offer another option:
Are you certain you know what you are doing? If you mark a pad as through hole then it will result in the drill file for plated through holes! Which means your manufacturer will not be happy with you. (And i would argue manufacturing takes precedence)
You CAN NOT see holes that are not plated. What you print/plot is COPPER.
as said, I make my own PCB’s. Thus… I am my own manufacturer.
When, in the past (perhaps before you were born) and used fab houses, my drawings contained manufacturing notes.
You ask, “Do I know what I’m doing?”
Answer: After 50 yrs of engineering (with degrees, patents, stuff flying is space and implanted in human bodies), I may not know what I’m doing but, haven’t heard complaints.
Below image shows two parts on pcb and quick milling setup in CopperCam (did not Horiz. Reverse it for this show&tell). Did not make any traces…
What you see is a BarrelJack with slots for flat tab-contacts and a Nokia 5110 LCD.
Thus, as said, it’s for my own needs. If what I’ve posted helps others to do something, great…
There is no such information in the post where you suggest to use plated through hole type to represent a non-plated hole.
If you include a disclaimer for something like that, then it is clear (Something like “danger this might not work if your PCB is produced by a modern fab”). A disclaimer at least adds a slight chance that a reader will not misunderstand your advice and use it in a case where it is inappropriate. Especially as the “i make my boards at home” usecase is really a minority at this point in time.
I just double checked with my system. Non plated holes show up as a faint circle if i select “real drill” for drill mark in the print dialog. If i select “Small mark” then they show up as a thick circle. And if i select “no drill mark” then i get a filled circle even for Mechanical (non plated through holes).
It seems to me the outer size of the circle always is the same size as the pad size (which should be equal to the drill size for non plated holes as that size is required for DRC as well). The drill mark selection only influences how large the “hole” is within that circle.
Tested with KiCad 5.1.5 under linux with the footprint MountingHole_2.1mm
I did point out it’s a thru-Hole/pad.
Commonsense should suggest S-DIP contains plated… and I clearly said a 'Thru-Hole pad.
I’m done…
This to me means you did not answer the question by @skybrian as they clearly asked how this should be done for non-plated holes. (The plated ones are already clearly shown in their printout)
My guess is you were unaware about the fact that non-plated holes and plated holes end up in different drill files and therefore could not foresee that your advice might be misunderstood.
Thanks, apparently “Small Mark” does what I want. I was misled by a previous discussion to believe that “Small Mark” wouldn’t show the holes as their actual size, so I didn’t choose that option.
It seems like the printing options could be clarified, so I filed a bug for this.
To be double sure we are all on the same page: The drill mark is the white area inside the black circle. The black circle represents the pad and is therefore controlled by the pad size. The drill size controls the white area (if you select “real drill”).
If you select “small mark” then you do not get the white mark with the size of the drill but as a small cirlce. This option exists to help users who etch their own boards as such a small mark helps centering the drill.
This is most clear on your other pads as “small mark” now really only leaves a small mark instead of the large white circles that were there in the past.
Maybe an option for “show non plated holes as thick outline” or similar could be useful for users who do not want to use the printout as a gateway for production but just as a way to see their work. (Or an option to mark drill centers with a cross)
I like the crosshairs idea.
As far as I can tell, for a non-plated mounting hole, the “pad” size is the drill hole size? It seems like you’re telling me it’s the wrong size when actually it’s the right size? It’s the other holes that are the wrong size?
I think I’m left where I started: not printing any circles for mounting holes when you asked for drill hole circles is confusing. The circles need to be thick enough for a laser printer to print. “Small mark” seems like a good workaround for showing mounting holes.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
