Silkscreen size - Page 1
Forum section: electronics / projects

author: IO390
author_rank: Regular Contributor
timestamp: July 28, 2014, 01:38:40 pm
content: Pretty simple question but...I'm working on a fairly dense PCB at the moment and I'm having trouble fitting in all the component labels.What would you guys say is the minimum readable size for PCB component labels (Silkscreen)?IO

author: Precipice
author_rank: Frequent Contributor
timestamp: July 28, 2014, 01:45:16 pm
content: I give up at 30 thou tall, 6 thou thick. They're legible at that size, with a good PCB house, but I mostly only bother with IDs for connectors and ICs now - there's never the space for passives.A build diagram, blown up to be legible, is far more useful, and the pick&place machines don't care one way or another...

author: uoficowboy
author_rank: Regular Contributor
timestamp: July 28, 2014, 02:35:25 pm
content: Most board houses can go down to 4 mil thick. Best to check with your board house. I've done 25 mil high, 4 mil thick and it came out pretty good but not for those with bad eyesight.

author: Precipice
author_rank: Frequent Contributor
timestamp: July 28, 2014, 02:44:07 pm
content: Most _good_ PCB houses are Ok at 4 thou. Bucketshops / pooling services, not so much, in my experience. Given how dangerous ambiguous idents are, and how little use they are most of the time, I err on the side of caution. If they're not fitting easily, they get hidden on another layer, and dumped dead central in the part, to make for a nice PDF build sheet.(Pin 1 identification, though - that's something I care quite a lot about!)

author: MagicSmoker
author_rank: Super Contributor
timestamp: July 28, 2014, 06:09:59 pm
content: Quote from: IO390 on July 28, 2014, 01:38:40 pm0.8mm is my default size for reference designators, but I have used 0.6mm for denser areas of a board and found it to still be readable without magnification, though barely so.

author: free_electron
author_rank: Super Contributor
timestamp: July 28, 2014, 06:55:42 pm
content: why put em at all ? if the board really is that dense simply don't put them. It;s going to be shot on by machine anyway.for hand assembly simply use a paper printout.

author: stef_r
author_rank: Contributor
timestamp: July 28, 2014, 07:43:34 pm
content: Wednesday I will receive my first PCB's made by a PCB house.I've done making my own for some small hobby projects, but since I had to scale up to a 4-layer board, that was just something I couln't do at home...Anyway, the smallest silkscreen size I've used is 32Mil for a 0603 resistor ID.See below:When I receive the PCB's, I will check the quality and readability of the silkscreen and post the answers of them, among with some pictures of the PCB.(I know it isn't Dave's favorite finisch, but it is 'painted Black'...

author: Precipice
author_rank: Frequent Contributor
timestamp: July 28, 2014, 07:59:55 pm
content: Crumbs, I remember when customers used to accept boards with spaces between componentsThis evening's job is trying to add some more stuff to this, without going to 0402 (it's mostly 0603 at the moment, for ease of homebuild). The back is equally full, but that's all optional goodies. I'm not losing sleep over the lack of component IDs.

author: IO390
author_rank: Regular Contributor
timestamp: July 29, 2014, 10:07:43 pm
content: Thanks for the replies. I ended up taking a sceenshot and labeling the footprints as suggested. Much more simple

author: T3sl4co1l
author_rank: Super Contributor
timestamp: July 29, 2014, 10:38:37 pm
content: I just did a run with 20 mil height, 4 mil line weight (Altium standard line font). Came out legible, though the hole in the "4"s is more-or-less closed over.American PCBs; YMMV elsewhere.An alternative to silk is to move all labels to a mechanical layer, and print that as an assembly drawing. In Altium, you can easily do this en masse: select all components, select their designators, then set auto-align center and layer to whichever mechanical layer.Tim