Pads doesn't support to output a complete NC route data, user have to use 3rd party tool for creating NC routing data.
If I am reading what you want correctly, you want a NP hole to pass an axial component (like a cap, diode, or resistor, or whatever) through before attaching, correct?
Are these parts completely or partially soldered to the board or to one or two other boards?
If soldered to the board, but also passing through it, simply add a third, non-plated pin (it would be pin 3) to the Decal. For a part tha only has one pin tied to the board, make pin 1 or pin 2 (whichever is appropriate) a 0-0, non-pated pin.
Otherwise, if the holes are simply there as a pass-through, either use the board cut-out you were already doing or a separate, possibly (or probably) non-ECO part that's just a non-plated hole, maybe with copper and other appropriate keep-out(s) built in to it. It can still have a designator, maybe something unique, like XCnn (I know it's non-standard, but as close as I can come to what would be appropriate, the "Cnn" part of the designator would correspond to the appropriate Cnn designator for the part).
Assuming you use attributes for things like description, part numbers, etc, I would give the pass-through only holes a part number of N/A or DNP, with the understanding with your assembler that anything listed as DNP or N/A is not placed.
Then use a description that maybe goes something like this (using a cap for this example): HOLE, PASS-THROUGH, CAPACITOR, n.nnn DIA **NOT A PLACED PART**
You could also use the "Assembly Varients" option so these parts won't show up in the BOM if you insist.
In this specific case I will be soldering the lead of an LED to a .100" square pad next to the hole. So in this instance I have a .100_PAD part in logic/layout. This is my generic solder pad for simple test boxes/prototypes. In some cases, I want to have NPTH next to this generic pad part. Like I said, I have solved this issue in the past but I was hoping for a "generic" solution at the Layout level. I bring this part up because I have used "board cut out" before only to receive a board with no cut outs.
I guess this brings me to a more generic question about the board cutout option. Should I expect the board manufacturer to know to cut out that section if I place it in the Drill Drawing and dimension it? I am not too familiar with the nitty gritty details of board manufacturing. I have attached a photo of what I'm attempting to do. This PCB will be mounted to the underside of a plastic test box. I want to slip the 2 axial lead diodes in from the other side and solder directly to the board. Is this all I have to do or should I be trying to get that cutout to appear on the NC drill file?
board.png 97.0 KB
If you have a cutout in the data, then yes, you should expect the fab to do it properly. However, I would dimension any cutouts in the fab drawing. I would also include a for-reference image of the board outline only, including any cutouts. The for-refernce image doesn't need any dimensions, just the board outline plus maybe a title block if you use them (See Image 1 below, Image 2 shows what I would put on the fab drawing).
As for your LEDs, I would build the cutouts in as a non-plated extra hole for these decals. This could be done as an alternate footprint for these parts, in case this is something you don't always do. Or, you could just have a separate Part/Decal for the LEDs with the extra hole. Your schematic symbol/Part doesn't have to have the NP hole shown, just make sure the Part name for the NP/non-NP parts have unique names so you know which one is being used.
Oops, I threw that image together very quickly, I just realized I left the hole diameters out for the stuff along the right edge. All of those cutouts are done with cutouts in the board, not NP holes.
Added new Image2 with the additional dimensions (poorly) added.
Message was edited by: jmatthews
For cutout, Fabs will generate NC routing data for those cutout if your drawing have drawn the profile and added notes. In China, every year there are ten thosands types of PCB with cutouts be fabricated, noone having NC routing data in thier original CAM data.
Expeditionpcb will automatically output NC routing data while generating drill tape, but Pads can't output any cutout data.