Missing pads in exported gerber file
100 11
Anson Mansfield 3 weeks ago
Here's the broken PCB layout: [https://easyeda.com/editor#id=da34a296559342849c6769dc1b87e409](https://easyeda.com/editor#id=da34a296559342849c6769dc1b87e409) When exporting the gerber files for manufacture, the center ground pads are missing on U13, U14, and U16, but _not_ on U15 - that pad is present, for some reason. This appears to be caused by the ground polygons I have surrounding underneath those chips, but all four chips including U15 have copies of this polygon. Deleting this polygon results in all four pads generating correctly, and for the moment I have replaced them in a different copy with simple traces to link the ground plane through the corners. This is actually a fairly serious problem, as I missed this in my manual check several weeks ago and ended up ordering a set of incorrect boards with the missing pads. My fault, I know, I should have checked harder, but this makes me a lot more wary about using this tool at all, if it's unable to reliably produce correct gerbers.
Comments
andyfierman 3 weeks ago
Have you checked the Gerbers using **gerbv** rather than the online checker at JLCPCB? [https://docs.easyeda.com/en/PCB/Gerber-Generate/index.html#Gerber-View](https://docs.easyeda.com/en/PCB/Gerber-Generate/index.html#Gerber-View)
Reply
andyfierman 3 weeks ago
Just rung the Design Manager on your PCB and it is flagging up lots of DRC errors on track width and clearances.
Reply
andyfierman 3 weeks ago
Yup, gerbv confirms the issue: ![image.png](//image.easyeda.com/pullimage/Z4xjiAbQcHk8L4yE6lqSGRLm5ZtV2YCC790hsrAB.png)
Reply
andyfierman 3 weeks ago
No idea why this should affect the Gerber generation but if I delete the devices and the solid regions I can see that there is a difference between how the copper area has built between U16 and the other 3 devices. The corners at 9 o'clock and 12 o'clock are not connected under U16 where as they are in the other three devices: ![image.png](//image.easyeda.com/pullimage/601ntNLuYzOloql4qcjCie7uwrP7VubI6FkC4tuT.png)
Reply
Anson Mansfield 3 weeks ago
@andyfierman The main reason for the large number of DRC errors is the differential USB traces, since EasyEDA doesn't let you set different clearance values for between a pair vs to other signals not in the differential pair, and most of the rest are about the package footprint escape areas.
Reply
Anson Mansfield 3 weeks ago
@andyfierman The upper of the two chips in your image still has the big copper polygon under it.
Reply
andyfierman 3 weeks ago
@anson.mansfield, @UserSupport, Exactly my point. The upper area in the EasyEDA PCB file has the pad in the Gerbers but the lower one, which is subtly different in the EasyEDA PCB file, does not but why that should affect the Gerber generation is something the developers need to investigate.
Reply
UserSupport 3 weeks ago
Hi Issue confirmed, please remove these solid region and add the track to connect the copper. we will investigate thie issue. Thank you very much ![图片.png](//image.easyeda.com/pullimage/pqODUkHKTuBbdHUX21h194zaoZNDL77eFKkQ86Lg.png)
Reply
UserSupport 2 weeks ago
After checking, it is a Gerber generate issue, if you move the solid region points to not to overlap for each other, it will correct. see the gap. we will try to fix it. thanks ![图片.png](//image.easyeda.com/pullimage/SYYPvT7ukT60EkOCWU5vfsPrhpuEG9FlrAWdGGRh.png)
Reply
Anson Mansfield 2 weeks ago
Ok, thank you, I suspected it's related to the pad being in the fully-enclosed empty region at the center of the polygon. I suspect the gerber exporter is interpreting the central pad under U13,14,16 as being fully inside their polygons and eliding it as "redundant"; while the difference in behavior for U15 may be due to some kind of difference in rounding behavior that causes it to not interpret that one as fully enclosing the pad. In my case, I _do_ want the copper to extend all the way around the pad, without a break in one side, and adding a noticeable seam is not ideal. If I split the polygon into two separate non-self-intersecting pieces that combine to make up the shape I want, will that allow the center pad to export correctly with the full filled region?
Reply
andyfierman 2 weeks ago
Or try creating a single solid region set to solid for the outer shape and then overlay a second solid region set to No Solid to define the shape of the inner, copper free area. Until the issue can he fixed, you need to think laterally about ways to achieve the desired result and try a few ideas.
Reply
Login or Register to add a comment
goToTop
你现在访问的是EasyEDA海外版,使用建立访问速度更快的国内版 https://lceda.cn(需要重新注册)
如果需要转移工程请在个人中心 - 工程 - 工程高级设置 - 下载工程,下载后在https://lceda.cn/editor 打开保存即可。
有问题联系QQ 3001956291 不再提醒
svg-battery svg-battery-wifi svg-books svg-more svg-paste svg-pencil svg-plant svg-ruler svg-share svg-user svg-logo-cn svg-double-arrow
We use cookies to offer you a better experience. Detailed information on the use of cookies on this website is provided in our Privacy Policy. By using this site, you consent to the use of our cookies.