You need to use EasyEDA editor to create some projects before publishing
Custom pads with partial solder mask in specific area
1196 6
hafridi21 4 years ago
Hi, I was wondering if it's possible to create a pad where a specific region is exposed, and the remainder is covered in solder mask (see photo below). I read a few related topics I could find on this forum, and it's giving me the impression that it may not be possible. I thought I'd ask to see if there is a workaround. ![AcroRd32_Qqy2wRwLT1.png](//image.easyeda.com/pullimage/D5AkhtwmCCAaLyrd94XYyboJtE0VahsZo4ckZcop.png)
Comments
hafridi21 4 years ago
I think I have it figured out in a round-about way...
Reply
hafridi21 4 years ago
I will post my method in case it helps someone in the future (or if I made a mistake or there is a better way, someone can point it out). The pictures below show a "test" footprint with the steps I used. ![easyeda_cphuFIqnLe.png](//image.easyeda.com/pullimage/zC2BnH60mFC3Ws6HCQMMXWtX7tpz7SIskil8g06Z.png) Result shown below (LED2) using the "Photo View" in a sample circuit. ![easyeda_QEDNHTfrp1.png](//image.easyeda.com/pullimage/CFIjsM1aNleYwr0YX32dmo1VTnZIBoMwdAPF0tsc.png)
Reply
andyfierman 4 years ago
Pads will always default to being exposed. There are at least 5 ways to do this. 1, 2 or 3 are "correct" ways to do it. $ and 5 are quick and dirty and may well come back to bite you. 1. 1. Make a PCB Footprint as in the right hand picture; 2. Edit the Solder Mask attribute to use a negative value so you can close the solder mask off (make it at least half the smallest dimension of the whole pad then make it negative); 3. Add 4 more top layer pads to the dimensions and positions of the left hand picture and give them the same numbers as the big pads they are going onto. 2. 1. Make a PCB Footprint as in the right hand picture; 2. Edit the Solder Mask attribute to use a negative value so you can close the solder mask off (make it at least half the smallest dimension of the whole pad then make it negative); 3. Add 4 Apertures in the Solder Mask Layer to the dimensions and positions of the left hand picture. 3\. \(I did make this work once but not sure I remember all the steps\.\.\.\) 1. Make a PCB Footprint as in the right hand picture; 2. Convert the pads to polygons; 3. Edit the polygons so that their centres are the centre points of the exposed areas; 4. Edit the Solder Mask attribute to use a negative value so you can close the solder mask off except for the exposed area of the pads. 4. 1. Make or find a PCB Footprint as in the let hand picture; 2. Route tracks to it on the PCB; 3. For each of the extended pad areas, add a Copper Area (set to solid not spokes) assigned to the relevant net name. 5. 1. Same as 1 but use a Solid Region set to Solid.
Reply
andyfierman 4 years ago
@hafridi21, Well done and thanks for posting your method! Our posts must have gone up at about the same time. :)
Reply
hafridi21 4 years ago
Thanks for replying @**andyfierman.** Looks like the first method you suggested corresponds to what I did, so I'm glad it's considered to be a "correct" one. Also, thanks for your contributions in this forum. You've posted a lot of info on other threads that I've found very useful.
Reply
andyfierman 4 years ago
Thank you. :)
Reply
Login or Register to add a comment
goToTop
你现在访问的是EasyEDA海外版,建议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 -mockplus- -mockplus- -mockplus- -mockplus- -mockplus- -mockplus- -mockplus- -mockplus-@1x -mockplus-

Cookie Notice

Our website uses essential cookies to help us ensure that it is working as expected, and uses optional analytics cookies to offer you a better browsing experience. To find out more, read our Cookie Notice