[Solved] Exposed Copper inside Circular Pad
123 9
bencfd 1 week ago
I created a footprint only composed of pads. The pads were converted from circular-shaped tracks. The 3D preview looks like what I am expecting, but the 2D preview shows that the inner part of the pads will expose the copper (after creation of the copper area). I was not able to reproduce the problem with only one circular pad, so I don't know what I've done wrong here. :/ Here is a public project showing the problem: [https://easyeda.com/bencfd/exposed-copper](https://easyeda.com/bencfd/exposed-copper)<br> <br> Any help will be greatly appreciated. Thank you in advance.
Comments
andyfierman 1 week ago
I'm not sure from your post but if you want the pads to **not** have exposed copper then apply a negative soldermask offset to the pads of at least half the track width. That will close the solder mask aperture over all the pads. Check the Footprint by placing it in a simple test PCB and then generating, downloading and checking the Gerbers using gerbv as recommended in the Tutorial. Do not rely on the JLCPCB gerber tools for checking.
Reply
bencfd 1 week ago
Thank you for your answer Andy. I'm having troubles installing gerbv, but I viewed the Gerbers using [http://mayhewlabs.com/webGerber/](http://mayhewlabs.com/webGerber/). It confirmed the problem visible on the 2D view of EasyEDA. I'm OK with the pads being exposed (that's on purpose), but the problem I have is that the solder mask aperture expands down to the center of this circular zone. I updated the project with a copper area to better demonstrate the problem (see picture attached). The copper area in the middle of the footprint gets exposed, which I would like to avoid.  ![Photo View_2021-01-10-2.png](//image.easyeda.com/pullimage/yKCMWE8BZaWE9s1bN7U0wM6wuq1wN2U445sp2ndn.png)
Reply
andyfierman 1 week ago
In the image above, there appears to be a copper area in the middle of the Footprint. If that is the case then it must be is a separate pad from the concentric structures so you can select that and apply a negative soldermask offset of at least the radius of that pad. However, your Footprint shown in: [https://easyeda.com/bencfd/exposed-copper](https://easyeda.com/bencfd/exposed-copper)<br> <br> has no centre pad. Can you post the url of the Footprint rather than the PCB you have placed it on?
Reply
bencfd 1 week ago
Indeed, there is a copper area in the middle of the footprint, ie inside the circular pads converted from tracks. It is built with _Copper Area Manager_, not from a pad, but it strangely gets exposed. Here is a link to the footprint, I hope it helps. [https://easyeda.com/component/52a7d0a0ad1c44bd9c4c0c06eaba7de2](https://easyeda.com/component/52a7d0a0ad1c44bd9c4c0c06eaba7de2) Thank you for your help!
Reply
andyfierman 1 week ago
This topic: [https://easyeda.com/forum/topic/How-to-avoid-DRC-errors-when-connecting-to-PCB-Footprints-a-k-a-PCB-Libs-90bf944fe3644b21a7d27a9e9d8df8d6](https://easyeda.com/forum/topic/How-to-avoid-DRC-errors-when-connecting-to-PCB-Footprints-a-k-a-PCB-Libs-90bf944fe3644b21a7d27a9e9d8df8d6)<br> <br> advises making **all** copper elements in a Footprint out of pads. If you modify the Footprint to make the inner circle of copper out of a pad then do the negative solder mask offset to cover it, that should do what you want. It will also create a Footprint that shows all its elements both in the Footprint Editor and when placed.
Reply
bencfd 1 week ago
I effectively followed this topic's advice and made all elements of the footprint out of pads. But I managed to isolate the problem. It comes from the outer circular pad. When it's about to close down to an entire circle, and when the (Top)SolderMaskLayer of the two tips of the arc overlay on one another, then the copper area gets exposed (**top** on the below figure; design is captured without showing the board's copper area). With more distance between the two tips of the pad, the copper area is not exposed (**bottom**). :) ![image.png](//image.easyeda.com/pullimage/N63e1xe3hiM2ppK2TgAOaoIgv9mW6lVZ3Otl0CXh.png)
Reply
andyfierman 1 week ago
OK, I understand how you've got the central copper now. Your work around seems reasonable but I think a centre pad with a closed off solder mask might be a safer option if you always want copper in the centre. It's a bit strange that closing the arc causes this issue (I think I have seen this before but cannot recall which topic...) but it's probably more of a "feature" than a bug worth reporting. BTW, did you find George Lepple's OS X packaged version of gerbv from here? [http://gerbv.geda-project.org/](http://gerbv.geda-project.org/)<br> <br> :)
Reply
bencfd 1 week ago
I tried a centre pad with a negative solder mask expansion, it works, yes, but I prefer to avoid this design because I want to place another component's pads in this area. I've found the package version of gerbv by Lepple, yes, but it requires fink, and it is not yet available for macOS 11. I registered to the mailing list to be informed when it will be available. ;)
Reply
bencfd 1 week ago
I edited the topic's title to mark it as solved. Thank you again for your help!
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.