JLC PCB - reorientation of octagonal pads - Page 1
Forum section: electronics / general

author: home_listening
author_rank: Contributor
timestamp: September 12, 2019, 03:21:40 am
content: Hi,Just wondering if anyone else has experienced this with JLC PCB, the rotation of octagonal pads has been adjusted by 22.5deg. Its fairly clear next to the clearance in the copper pour of this board. Not a big issue on this order as its a mounting point for heatsinking, but for closer tolerance designs it could be a major problem. I've emailed them about it.Cheers -HL

author: Mangozac
author_rank: Frequent Contributor
timestamp: September 12, 2019, 05:46:00 am
content: The image won't load for me, but I'm curious the reason for selecting octagonal pads over round?

author: Eunice Yin
author_rank: Newbie
timestamp: September 12, 2019, 05:56:10 am
content: @home_listeningI don't think this is a problem of them, maybe the problem of your Gerber file generation software.

author: JLCPCB Official
author_rank: Regular Contributor
timestamp: September 12, 2019, 06:57:47 am
content: @home_listeningDear Sir,This is JLCPCB support, we are very sorry that there is a problem with your order.Generally we can't any modification with customer's design without the permission of customers. And if there is any design modification requirement, we will ask our customer to modify it by themselves in case there is any misunderstanding.Regarding your problem, We can not help to check out where the problem is, since We don't know your order number. Could you pls send email support@jlcpcb.com or submit a complaint on JLCPCB account, they will solve the issue soon.If it is our problem and you can not use the board, we will refund or remake the board for you, so please don't worry, haha.We consulted our engineer, they said there maybe a bug when you generate the Gerber file.Any question,just feel free to contact with us

author: home_listening
author_rank: Contributor
timestamp: September 12, 2019, 07:11:44 am
content: Quote from: blueskull on September 12, 2019, 04:11:09 amYeah, I did the PCB in eagle and checked it in the Kicad Gerber viewer and then the JLC websites gerber viewer - all of these show the correct orientation. So it happened somewhere down the line.

author: home_listening
author_rank: Contributor
timestamp: September 12, 2019, 07:14:09 am
content: Quote from: Mangozac on September 12, 2019, 05:46:00 amI suppose I could argue that the geometry of the octagon offers slightly greater surface area on the pad compared to a circle, but to be honest I just like the look of a bunch of 45degree traces next to the 45degree angles of the pads.

author: home_listening
author_rank: Contributor
timestamp: September 12, 2019, 07:15:28 am
content: Quote from: Eunice Yin on September 12, 2019, 05:56:10 amThe pads are the correct orientation in my software, when viewing the gerbers in Kicad's gerber viewer as well as the JLC website gerber viewer. Since you are clearly a bot, perhaps stick to more honest tasks like trolling Justin Biebers twitter account?

author: home_listening
author_rank: Contributor
timestamp: September 12, 2019, 07:16:53 am
content: Quote from: JLCPCB Official on September 12, 2019, 06:57:47 amI appreciate the response, This isn't a big problem for me on this project - I didn't even notice until today (a month or so after I got the boards) and everything built so far has been fine. I reported the bug through the website today so it should show up for you.Cheers.

author: xavier60
author_rank: Super Contributor
timestamp: June 04, 2020, 01:33:11 am
content: PCBWay can do octagonal pads correctly from my Protel 98 PCB files.They have to be reminded to check otherwise there is a chance of the octagonal pads being converted back to round at production time.I have never been able to produce my own Gerber files with the octagonal pads showing correctly. They either get converted back to round or are rotated by 22.5°.I got a reply from JLCPCB saying "Gerber only"

author: phil from seattle
author_rank: Super Contributor
timestamp: June 04, 2020, 04:41:52 am
content: Interesting, they appear to still be doing it. Or I should say, doing something similar. I hadn't noticed until I read this (old) post and looked at my recent boards from them. I'm trying to attach a photo of it but not seeing it on the preview. If it shows up, you can see that they have rotated the octagonal pads by almost 45 degrees. They didn't change the copper around the pads so you can see what I originally intended. I also tried to attach a image of the board design to show what I wanted. Pretty sure my DRC would hurl lunch over the rotation because it's less than 6 mil clearance. I've had several boards from them and they seem to work fine. Maybe I should switch to round pads. Eagle 7.7

author: xavier60
author_rank: Super Contributor
timestamp: June 04, 2020, 04:50:23 am
content: Quote from: phil from seattle on June 04, 2020, 04:41:52 amIs the problem visible when your Gerber files are viewed?

author: phil from seattle
author_rank: Super Contributor
timestamp: June 04, 2020, 05:28:33 am
content: Good question. No, they appear to have the correct orientation. Though, the JLCPCB gerber view isn't very clear so I have been relying on other gerber viewers. I haven't had any other issues with them. [edit: all other viewers show the correct orientation]I've had 3 PCBs made by them and all of them have the same issue. Though, the first two have been fully validated with no errors (design or fab) and I am in the process of validating the third - it looks very solid as well. Other than the issue being discussed. I've attached a screen shot of approximately the same area from their website. A little hard to make out but the pad orientation looks correct.

author: JLCPCB Official
author_rank: Regular Contributor
timestamp: June 09, 2020, 03:25:10 am
content: Quote from: phil from seattle on June 04, 2020, 05:28:33 amhello sir, do you mean by our Gerber view is not good?any suggestions for our " JLCPCB Gerber view "

author: phil from seattle
author_rank: Super Contributor
timestamp: June 09, 2020, 08:46:57 pm
content: Thank you for replying. The gerber shown is small and the gerber viewer is clumsy to use (zoom interface in a small window).Note that for the purposes of the above discussion, there wasn't an easy way for me to get to the view for the project that had been completed.I just went and uploaded my old project and used the gerber viewer to check the project I submitted (the one with the rotation issue) and the JLCPCB viewer shows the octagonal pads as properly oriented while the PCBs I received have them rotated by about 40 degrees. While I continue to be a customer of JLCPCB, I am concerned that the board was not what I had expected. I have changed to use round via's and pads to better work with your processes but wonder why this happens. Other vendors do not have this issue.

author: JLCPCB Official
author_rank: Regular Contributor
timestamp: June 09, 2020, 09:57:20 pm
content: hello ;Good that you have Emailed the issue to the technical team first, in the EDA you are using you can manually set the component orientation by rotating it through a customized rotation angle so no need for the automatic rotation since it depends on each components.

author: phil from seattle
author_rank: Super Contributor
timestamp: June 11, 2020, 07:49:36 pm
content: Quote from: JLCPCB Official on June 09, 2020, 09:57:20 pmYes, true for components but there is no way to change pad or via orientation - they are not components.

author: oPossum
author_rank: Super Contributor
timestamp: June 11, 2020, 09:41:42 pm
content: Octagonal pads can be rotated in Eagle in the library editor but this should not be necessary. I have had 3 PCB designs done in Eagle 7.7 made by JLC and they all had the correct pad rotation. A picture of one is attached.

author: phil from seattle
author_rank: Super Contributor
timestamp: June 12, 2020, 12:49:01 am
content: Sure, but there is no way to do it through their interface. And, frankly, it would be a terrible service if I had to redesign a part each time I try to get a board made - the rotations do not seem to be consistent from job to job. And finally, their gerber viewer doesn't show the way it will look when manufactured so there is no way to know the rotation needed, a priori. and in Eagle, there is no way to rotate a via, square or octagonal.

author: xavier60
author_rank: Super Contributor
timestamp: June 12, 2020, 01:21:44 am
content: Futurlec used to send me a PDF file showing exactly what the layers were going to be like for my approval before production.I often had to point out the presence of octagonal pads. They would always eventually get it right.

author: oPossum
author_rank: Super Contributor
timestamp: July 03, 2020, 11:48:12 pm
content: My previous three JLC orders all had correctly rotated octagonal pads, so I ordered eighteen different PCBs designs a few weeks ago. All of them have at least a few octagonal pads. They arrived a few days ago and results where not as expected. Eight have the correct rotation and the other ten are incorrect. Several of these used the same library part (40 pin 0.1 header) and began as the same schematic/PCB template. I thought the Eagle CAM file may have been the cause of rotated pads but this is clearly not what is happening. Something is very wrong with the CAM processing at JLC. Here is a link to a picture showing a PCB from ~6 months ago that is correct (top), and 7 from the recent order with only one correct (2nd from top):http://compendiumarcana.com/forumpics/jlc_oct.jpgThere may also be some drill size and/or pad size problems (not shown in that pic). I haven't measured that yet, but it doesn't look right.

author: xavier60
author_rank: Super Contributor
timestamp: July 04, 2020, 12:25:40 am
content: It's a very puzzling problem.If I generate my own Gerbers from Protel 98, I see some 22.5° rotated octagonal pads when I check with a viewer.

author: phil from seattle
author_rank: Super Contributor
timestamp: July 04, 2020, 01:30:07 am
content: Yeah, it's a bit of a mystery. I simply stopped using octagonal pads for JLCPCB boards. I'm a little dissatisfied over it - I prefer octagonal because they make it easy to avoid acid traps. But, for the cheap service, I'll live with it.

author: JLCPCB Official
author_rank: Regular Contributor
timestamp: July 04, 2020, 02:09:28 am
content: Quote from: home_listening on September 12, 2019, 03:21:40 amHi. SirSoftware compatibility problems causing this angle to shift. We received feedback and have improved this kind of octagonal pad problem, which has greatly reduced the occurrence of similar situations. You should receive a reply email as soon as possible and hope you get a satisfactory reply. thank you!

author: IconicPCB
author_rank: Super Contributor
timestamp: July 13, 2020, 10:28:57 pm
content: I seem to recal the old Protel software had this kind of feature.Some pads would not translate well from Gerber to photo tool.Altium has not had this problem to the best of my knowledge.Just to round off... The problem is not necessarily with JLCPCB CAM software, it is more likely to be with individual clients Gerber exports.

author: Lukas
author_rank: Frequent Contributor
timestamp: July 13, 2020, 10:48:47 pm
content: Try opening your gerbers in CAM350 (demo version works) since that's what they use at JLCPCB. That wouldn't be the first time that CAM350 misinterprets the gerber spec:https://blog.horizon-eda.org/misc/2019/11/18/gerber.html

author: phil from seattle
author_rank: Super Contributor
timestamp: July 14, 2020, 06:09:22 am
content: Well, I can't say for other software but I seriously doubt this is Eagle's fault. The JLCPCB gerber viewer shows correct orientation of the pads. And, I've used most of the other popular board houses - PCBWay, ALLPCB, Seed, OSHPark, and several others on at least 60 different designs. None of them have had this issue. Every Gerber viewer I've ever used shows the pads correctly. I've been getting PCBs made for around 14 years now and have never even heard of this problem until now.

author: xavier60
author_rank: Super Contributor
timestamp: August 04, 2020, 02:12:23 pm
content: "Octagonal pads are rotated by 22.5 degrees in gerber plots. Most australian manufacturers then rotate them back again for you"fromhttps://airborn.com.au/layout/autotbug.htmlMaybe some manufacturers are correcting octagonal pads that don't need to be.

author: mkstevo
author_rank: Newbie
timestamp: January 15, 2021, 06:16:58 pm
content: I've had this problem in the past. An order was delivered with the large octagonally plated screw holes I'd added rotated, the points of the octagon just connected the copper plane to the screw hole/via. This caused the top copper plane to become shorted to the bottom copper plane, creating a short circuit between 5V and 0V. I like to have a large plated area around any screw holes as it helps me to visualise the screw heads or stud dimensions so that I can avoid running tracks close to any screw holes, avoiding the risk of a screw being able to connect to a track and create a potential short if that screw is over tightened. I have, since this experience, made a note not to use octagonal pads for any drill holes.I use Eagle 7.7. On exporting the designs to Gerbers, I often check them usinghttps://tracespace.io/view/I sometimes also use an offline Gerber viewer for macOS too. On the particular design that caused me problems I wondered if I'd made a mistake, I triple checked it with as many Gerber viewers as I could and none of them rotated the octagonal pads for either the vias I used as screw holes nor the resistor and capacitor pads that are the default shape for Eagle. All had been rotated on the boards made by JLCPCB.I'm not saying that it wasn't an export issue by Eagle, but as every Gerber viewer I tried showed the correct orientation it seems possible that there may be a formatting problem or mismatch with how JLCPCB process octagonal pads.On raising the issue with JLCPCB they re-manufactured the boards free of charge. I changed the hole shape to round before submitting the file for a second time. Just in case.Either way, as I have no problem with the rotated pads for resistors and capacitors shorting to my copper planes it hasn't caused me any further failures.On the most recent designs I have not seen this issue on the resistor or capacitor pads, although reading this thread it seems to appear at random intervals and not always on all boards in the same batch.

author: atommann
author_rank: Newbie
timestamp: January 16, 2021, 11:42:14 am
content: We've figured out how this issue happened at JLCPCB and I try to explain it in this post.Octagonal pads and vias are very common in Eagle. When Eagle outputs Gerbers, an aperture macro called OC8 is used to represent these pads and vias.Code:%AMOC8* <1>5,1,8,0,0,1.08239X$1,22.5* <2>%%ADD10C,0.00700*%%ADD11C,0.00300*%%ADD12R,0.47244X0.19685*%%ADD13OC8,0.06000*% <3>Start to define the OC8 macro, AM = Aperture MacroThe contents of OC8, primitive code 5 means Polygon, 1 means Exposure On, 8 means octagon, 0,0 is the x/y coordinate of center point, 1.08239X$1 means Diameter, 22.5 is the rotation angle.This line defines an aperture D13, it uses macro OC8.This figure below is from The Gerber File Format Specification November 2013 Revision J1https://web.archive.org/web/20130630231317/http://www.ucamco.com:80/en-us/downloads.aspx, page 92, which is about primitive code 5 (polygon).Note: In newer Eagle versions (such as 9.6.2), the octagonal pads are output as standard Regular polygon, macro OC8 is still in the file, but it not refered anymore. Here's a related threadhttps://forums.autodesk.com/t5/eagle-forum/gerber-regular-polygon-add-lt-nr-gt-p-vs-add-lt-nr-gt-oc8/td-p/7864702Code:%ADD32P,1.649562X8X112.500000*%In the CAM tool which is used to process the Gerbers, there is a parameter called: xxx_set_octagon_rot, it has two options:* no - starting rotation angle of an Octagon = 22.5 (default)* yes - set it to 0Now, if this xxx_set_octagon_rot = No:It means "starting rotation angle of an Octagon = 22.5 (default)", we can know its starting rotation angle, it's like this:Because OC8 has a 22.5 parameter, so when the CAM reads in the Gerbers, all octagonal pads will be rotated 22.5 degrees (the right one in the above figure will be used as the template), and we get the wrong angles as the users reported in this thread.If this xxx_set_octagon_rot = Yes:"yes" (set it to 0): This is the same with the definition in Gerber spec, in this case, one vertex is on the horizontal axis x. When the CAM tool reads in the Gerbers, it just rotate octagonal pads by 22.5 degrees, this is just the rotation angle in Eagle and customers will get the right boards!On Dec 29 2020, JLCPCB upgraded the system just for this issue, to prevent this issue from happening in the future: Every file will be scanned for these OC8 macros, and the person who processes these Gerbers will be warned that these designs have octagonal pads/vias.This afternoon (Jan 16, 2021), I placed 20 true orders (Eagle 7.7.0 with the arduino example) in JLCPCB's website and got the process "ok" file, the rotation angle for octagonal pads in all "ok" files are correct.PS: Don't know how to insert the inline images. I need the help from the moderator. Thanks.