Printing PCB Design? - Page 1
Forum section: electronics / general

author: theatrical scene
author_rank: Contributor
timestamp: January 22, 2019, 10:42:04 pm
content: I'm just wondering how I can print out just the outline of my PCB so I can see if it fits my enclosure? Following the instructions here:https://www.altium.com/documentation/18.0/display/ADES/((Configuring+PCB+Printouts))_ADI can only print the components rather than the board outline. Is there something I'm missing?

author: ajb
author_rank: Super Contributor
timestamp: January 23, 2019, 01:51:50 am
content: It's on the page you linked under "Configuring 2D Print-based Output". You can select whatever layers you want for a given printout, so if you want just the outline, you'll need to make sure that you have the outline in a distinct layer. You should likely also put center marks for any mounting holes in a mechanical layer so you can make those print as well.

author: theatrical scene
author_rank: Contributor
timestamp: January 23, 2019, 02:28:57 am
content: Quote from: ajb on January 23, 2019, 01:51:50 amThanks, maybe that's my issue then! How do I change the outline to be on a distinct layer? It currently appears as 'Multi-layer' in the board planning view, should I draw the outline again with another layer e.g. "Mechanical 4"?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 23, 2019, 04:00:02 am
content: Usually, Keep-Out Layer is used for outline, or Mechanical 1 nowadays. Whatever it is, put the outline on that layer, select it and D, S, D (Design / Board Shape / Define from Selected Objects), and there's your outline and the layer it came from. Then generate that layer in the OutJob or whatever.Mind that PCB PDF output is crap for scaling and you may have to customize the border / scale / outline to get it to line up right. Use a vector format (i.e., Gerber) with an appropriate viewer/driver to get proper scale.Tim

author: ajb
author_rank: Super Contributor
timestamp: January 23, 2019, 05:19:33 am
content: Tim makes a good point about the scaling issue. You might have better luck with Draftsman, but I haven't messed with it much. I mostly use PCB->PDF outputs for reference drawings where scale isn't an issue.Other things that are useful to know when interfacing with mechanical design factors:- You can actually create a 2D outline by slicing a 3D object, so you can actually import a 3D model of your enclosure, position it height-wise relative to your PCB, and then generate an outline that way (obviously it's on you to provide the required clearances)- You can import and export DXF/DWG, which can be in turn be exported and imported by a lot of vector graphics programs (CorelDraw, Illustrator, Inkscape) as well as CAD programs. This can be very useful, as DXF is a nice common denominator for 2D mechanical information.

author: free_electron
author_rank: Super Contributor
timestamp: January 28, 2019, 02:07:32 pm
content: Quote from: T3sl4co1l on January 23, 2019, 04:00:02 amdo not use the keep-out layer for the board ontour!. since AD17 that has changed.Keep out layer is really for that: keep out.The boar dcontour is defined in board outline. it is no longer a separate layer.

author: theatrical scene
author_rank: Contributor
timestamp: January 28, 2019, 10:28:42 pm
content: Ah ok. Some of my components use Mechanical 1 as silkscreens, would I need to remove these/change layers if I were to make the outline using Mechanical 1 (not just for printing but also for Gerber generation to send to the fab)?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 29, 2019, 12:20:37 am
content: Probably a good idea; just query:OnLayer('Mechanical 1') AND NOT IsFreeand in Properties, change them to another mechanical layer.This fixes it on the PCB, assuming you never update from libraries. To fix those, open each PcbLib and do the layer query (don't need IsFree, it's all free) for all components, and change them en masse.Tim

author: theatrical scene
author_rank: Contributor
timestamp: January 29, 2019, 12:54:11 am
content: Many thanks for that! Absolute legend Tim.

author: ajb
author_rank: Super Contributor
timestamp: January 29, 2019, 04:35:52 pm
content: Quote from: theatrical scene on January 28, 2019, 10:28:42 pmAltium provides dedicated layers for silkscreen: Bottom Overlay and Top Overlay. These are what get rendered in 3D view, and they get the standard GTO and GBO gerber extensions by default, so it's a good idea to use them. In AD18 and earlier you had to use Mechanical layers for basically everything except copper, silk, and paste. There were conventions as far as which layers to use for which purpose, but there was nothing to really enforce those conventions. AD19 now has explicit component layer pairs for 3D Bodies, courtyard, designator, etc, which should make things a bit easier to deal with, at least once component libraries get updated to use them.Quote from: free_electron on January 28, 2019, 02:07:32 pmWhat do you mean by this? Is there some new way to define a board outline without using the standard line/arc primitives in a mechanical layer?(I know you can define from a 3D body, but I don't particularly like the lack of control over the mechanical interface this provides. Also obviously Altium represents the board outline internally separately from the primitives that were used to define it, but I don't know of a way to initially define the board outline without some sort of mechanical primitives (D,S,D).)

author: twistedresistor
author_rank: Contributor
timestamp: February 11, 2019, 06:35:29 am
content: Quote from: ajb on January 29, 2019, 04:35:52 pmIs there a document which layers they used for what?

author: ajb
author_rank: Super Contributor
timestamp: February 11, 2019, 04:39:01 pm
content: Quote from: twistedresistor on February 11, 2019, 06:35:29 amI thought the new layers were separate from the mechanical layers, but looking at it more closely it turns out this is not the case. They still need to be assigned layer numbers, so AFAICT what's actually happening is that the new component layer pair dialog just assigns them more meaningful names. I'm not sure if this changes anything as far as layer selection in filter/rule queries or outjobs or whatever. This also means that Altium does not enforce any rule or convention on which layer (numbers) are used for what purpose. I've always used this convention:https://blog.mbedded.ninja/electronics/general/altium/altium-tricks-and-standards/#pcb-layer-standards

author: ddavidebor
author_rank: Super Contributor
timestamp: February 16, 2019, 07:38:47 pm
content: You could try Altium Draftsman - place a single layer board view - with an empty layer. it will print the outline. You can select the sheet size to whatever your printer supports.