What happens on the Outline layer? - Page 1
Forum section: electronics / general

author: rokask
author_rank: Newbie
timestamp: June 09, 2024, 08:49:36 pm
content: Good day,I've made the sad mistake of learning how to use CircuitMaker (Altium's differently-abled step child) and with my current project (2nd overall) realized that it's an abandoned piece of software. Will be moving to KiCAD for my next one, but please see if you can help me out with understanding a particular design concept:What is the Outline layer used for (see attached picture)?From reading the ample Altium forum conversations, it seems like the equivalent of what mechanical layers are on the good software. All I know is that this is where I place the outline for my board cutout so that PCBway stops rejecting my project. My concern today is that a 3 pin XH 2.54mm connector has placed it's own scribble onto the outline layer. Will my board get cut there? Couldn't find a way to remove it without replacing with a similar component. I know that the "Drill drawing" layer is how you ask for holes to be cut into your project. What will the blue square in the middle of my board do if I send it in?

author: ataradov
author_rank: Super Contributor
timestamp: June 09, 2024, 09:26:58 pm
content: When sending files to PcbWay, send the Gerbers and name the Gerber files according to their requirements. It does not matter how they were named in the original project.If you supply this as the actual board outline, then they will likely reject it. No idea if there is an actual board outline layer already, if not you either need need to make one, or edit the component to remove that stuff.

author: ajb
author_rank: Super Contributor
timestamp: June 09, 2024, 09:37:06 pm
content: You might get more help in the CircuitStudio forum, since that’s more closely related, but not sure how active it is.QuoteIt should be used for the actual outline of the board. Some people use the ‘keepout’ layer in Altium, and sometimes the .gko file extension for the corresponding gerber, but that’s logically a different thing with a different purpose. The outline layer should include all of the edges of the board, including internal edges around holes. Some fabricators request you mark internal cutouts specifically, ie “CUTOUT” text inside of the cut outlines, but I think generally they’ll assume that’s what you want. But if they see tracks/pads/vias inside of those outlines they’ll flag it, since they assume you probably didn’t mean to route through those features.QuoteSort of. As above, holes *routed* into the board should be in an outline layer. The drill drawing layer is for documenting *drilled* holes, but since all of the necessary fabrication data for drilling is generally present in the NC drill files, it’s not often used. It might be useful if you’re doing boards with blind/buried vias or some other very particular fabrication requirements, but I don’t make those sorts of boards and have never used it.*In the PCB component properties, is there an ‘unlock primitives’ option? Or maybe in a context menu? In Altium, that would let you select the primitives in the footprint and delete them without having to go in to the library and edit them there.Alternatively, you could use a different layer for your board outline and generate your outline gerber from that. There’s no real difference between the gbl, gtl, gbo, etc gerber files in terms of formats, it’s just a naming convention. So as long as you can get a gerber with the right data out of the software you can freely rename it as needed before sending to the fabricator.*OT, but I actually have a hard time imagining a scenario where a drill drawing is useful given modern boards and fabrication methods. CAM tools don’t need a visual representation of what size holes to put where, just a list of coordinates and sizes is fine. Same for inspection tools, or for planning blind/buried stackups. It’s not like humans are doing the drilling, or even closely supervising the drilling, these days! Maybe if you want a visualization of how different drilling operations/hole types are distributed over a board for DFM or process optimization purposes, but I expect CAM tools can do that better from the machine-readable listings as well, with interactive filters and so on. But I don’t know — maybe I overestimate the capabilities of modern CAM tools

author: exmadscientist
author_rank: Frequent Contributor
timestamp: June 09, 2024, 09:43:08 pm
content: Quote from: ajb on June 09, 2024, 09:37:06 pmIMO the only thing a drill drawing is good for is spot checking. "Yep, our CAM software has about the same spread of drill holes as that drawing." This would catch brain-dead errors like using the wrong units for the drill file, etc.You might think that sounds useless, because you might think there are so many other ways to accomplish the same thing. And perhaps youshouldbe right. But there are some really, really careless fabrication shops out there....These days I don't bother with a separate drill drawing or drill Gerber layer. But on my fab drawings I always have the board outline, and I just turn on showing the drill hits inside that outline. Simple, obvious, and works well. It also gives me a natural place to put a drill table, and having a drill table can be very useful to whoever is quoting your job.

author: rokask
author_rank: Newbie
timestamp: June 09, 2024, 09:54:46 pm
content: Quote from: ajb on June 09, 2024, 09:37:06 pmYusss!! You were right, there is an option to unlock primitives for the item and remove them selectively.Thank you all for your inputs, I can see you talk from a place of understanding but I am yet to get there.