pcb woes jlcpcb npth with traces - Page 1
Forum section: electronics / general

author: tablatronix
author_rank: Regular Contributor
timestamp: May 26, 2018, 03:31:10 pm
content: using eagle, trying to generate mouse bites with traces.JLCPCB keeps rejecting my order, but I am failing to see why, or where they are getting these failures from."As shown below, the holes makes the lines drilled off"I have .25 mm drill hits, with ~.25mm hole to trace, 6 mil traces.min drill is .2mm on their capabilities.Of course an email conversation with them takes 2 days because of timezone.I am probably pushing my luck here, and should just use another fab house, but I thought I would try one more time.eagle 1mil gridlast image is their screenshot, It looks like they are upsizing my holes, or calculating them from profile/outline wrong even though they are in the drill file. baffled.

author: tablatronix
author_rank: Regular Contributor
timestamp: May 26, 2018, 03:35:32 pm
content: full stackup

author: matseng
author_rank: Frequent Contributor
timestamp: May 26, 2018, 03:51:44 pm
content: To me it looks like the holes are too close to the cutout - at least that is what the arrows points to. Some fabs don't like to make holes (and/or copper) close to the board edges...

author: tablatronix
author_rank: Regular Contributor
timestamp: May 26, 2018, 04:10:43 pm
content: Possibly, in my gerbers the cutout is >0.2mm from holes and within capability listed.But the email said "As shown below, the holes makes the lines drilled off"Which makes no sense to me from my gerbers, even accounting for drill tolerance of ±0.08mm.It is like they are not using profile midline?

author: matseng
author_rank: Frequent Contributor
timestamp: May 26, 2018, 05:05:35 pm
content: How wide is your cutout? I've discovered that many cheap fabs uses what looks like a 1.2mm or even 2mm router bit for the internal slots. This might expand the slot on your pcb and make the edge too close to the hole.

author: tablatronix
author_rank: Regular Contributor
timestamp: May 26, 2018, 05:33:01 pm
content: I think its about 1.2mm but this rejection is the same as last drills will cut traces. The i made holes smaller and added tons of space and still their screenshot does not match my holes.I dont think cutout is the problem but i will ask them.

author: DerekG
author_rank: Frequent Contributor
timestamp: May 26, 2018, 10:26:54 pm
content: Quote from: matseng on May 26, 2018, 03:51:44 pmI would agree. The board shop may mill to the centre of your rectangular (with rounded corners) cut out line, while others will mill right to the outer edge of the line. I personally would have chosen a narrower outline for the cutout (remember it is normally shown on a mechanical layer, not a copper layer).So, I agree with matseng in that your cutout is too close to your existing pad holes.

author: HwAoRrDk
author_rank: Super Contributor
timestamp: May 26, 2018, 10:47:52 pm
content: Wait, are your mousebite holes in both the mechanical (i.e. board outline) layer gerber fileandthe drill file? They should only be in the drill file. So if they're trying to route them according to the outside of the lines in the GML then it's unsurprising they're complaining because it looks like it will cut the board completely in two due to the overlap.The only other thing I can think of is that you didn't put these NPTH in a separate drill file, so they are treating them as plated, and so expanded the hole size to accommodate the plating thickness.

author: tablatronix
author_rank: Regular Contributor
timestamp: May 26, 2018, 11:25:29 pm
content: Yes thank you , I was wondering that also.So I am wondering why does eagle cam processor put npth in mechanical (board layout,cutouts) ?(jlcpcb site specifically says "Please use Outline to design if there are many non-plated (NPTH) holes." ) So I assumed they would deal with this fine by comparing the 2.Maybe I just need to make eagle not put these drills in mechanical somehow.Any Ideas?

author: tablatronix
author_rank: Regular Contributor
timestamp: May 26, 2018, 11:32:27 pm
content: I guess I will try to just use board outline and milling layer and try that...

author: tablatronix
author_rank: Regular Contributor
timestamp: May 26, 2018, 11:42:21 pm
content: Also I have no idea what dictates the line thickness in the mechanical layer that the cam processor generates when you click cutouts and board outline, Those are not line widths I have set, but maybe I have them set to 0 so they are defaulting.

author: tablatronix
author_rank: Regular Contributor
timestamp: May 28, 2018, 02:07:56 pm
content: Well no rejection this time, Thanks for your help, eagle 9 cam cutouts checkbox auto includes npth holes in mechanical, I have no idea why they do that.

author: HwAoRrDk
author_rank: Super Contributor
timestamp: May 28, 2018, 07:00:03 pm
content: Excellon drill format includes support for slotted holes, but some PCB manufacturers don't support that, so in that case one needs to put these holes in the board outline gerber to be routed out that way.

author: tablatronix
author_rank: Regular Contributor
timestamp: May 28, 2018, 08:25:46 pm
content: Yeah I am reffering to all npth of any size. I have asked in their forum why this is, id expect this behavior for drill sizes but not in drills or slots. Seems like an odd feature.

author: vipcircuit.com
author_rank: Newbie
timestamp: June 28, 2018, 08:05:32 am
content: npth to line 0.25mm, line width 6mil, seems no problem