moving items from document layer to silkscreen layer
55 6
glenp 1 week ago
I have some panel mount potentiometers where the pads for the pots are in the right layer, but the outline of the pot itself is on the document layer.  I'd like to move these to a silkscreen layer, but there is no way to select them/ move them.  How can I do this? Thanks!
Comments
andyfierman 1 week ago
Can you post a link to the footprint?
Reply
glenp 1 week ago
link is here:   [https://easyeda.com/glenp/proco-rat](https://easyeda.com/glenp/proco-rat) I'm referring to the big 3 pots in the middle.  I want the "drawing" of the pot to be on the bottom silk layer, not the top, like the jacks above them. Note- i'm just learning pcb design, so i know the routing is a bit wonky :)
Reply
andyfierman 1 week ago
Note that you can't edit the footprint that has been pulled into the PCB. You have to edit the PCB Lib i.e. the PCB footprint in the library. For more on this please see: [How to create findable Footprints and searchable Symbols.](https://docs.google.com/document/d/e/2PACX-1vRBxS8uUSbskSIrJrNabh0A8qp0gZmWfUG7GlXX7oltY6XC9dukqS_BU-w4F-UarCNydPWOYz10VQ5V/pub)
Reply
glenp 1 week ago
Thanks Andy!  what I'm doing is creating my own personal library (footprint/schematic) and then updating how it looks.  This seems to be working well- I can update the schematic with the new version, and then update the PCB from there.
Reply
andyfierman 1 week ago
Thanks but I was after a link to the pot PCB Footprints rather than you particular project. Try just entering the name in the search box in the top left of the forum page or in your User Centre page.
Reply
andyfierman 1 week ago
@glenp, Looks like you have edited the PCB Footprint to create your own. ![image.png](//image.easyeda.com/pullimage/WRvHVsoM3KeO7H9NUWc73MHMqwyb4xcJr5aTW2uP.png) However, you have created a footprint as seen looking from the top layer through into the bottom layer. That is not the right way to do it. * PCBs are always viewed looking down on the top layer and that layer is assumed to be the component side for through hole components (and usually for SMD too). * All PCB Footprints are created for the part mounted on the top layer of the PCB so if you look at the PCB it is mounted on the top side facing you. * If you want the part on the underside of the PCB then you put it on the top layer and then swap it from the top to the bottom layer after placing it. * Designing footprints for the bottom layer will cause confusion because everyone expects them to be designed for mounting on the top layer and then flipped onto the bottom layer. The only possible exception might be if you want a pot to be mounted on the PCB from the underside, with the shaft passing through a hole in the PCB and the mounting pins inserted from the bottom of the PCB. Like this: ![Reverse Type High Power B500k Rotary Dual Gang Potentiometer](https://image.made-in-china.com/201f0j00TOgQmFkPhYcH/Reverse-Type-High-Power-B500k-Rotary-Dual-Gang-Potentiometer.jpg) If you deviate from the rules above you MUST add notes in the Document layer of the footprint to make it clear what the deviation is. Otherwise someone will pick it up, put it on the top layer and whether they flip it or not,, it will end up wired back to front. I suspect that this is what you want: ![image.png](//image.easyeda.com/pullimage/V8RrWJwqckEwOIAXq2FpQFaGsCI5nWOTyXv1fWOq.png) Which if you open it in the editor will show you that it has a silkscreen on the top and the same outline in the Document layer too: ![image.png](//image.easyeda.com/pullimage/JjYUTw0jRqD5mmdaMcBn2nVvJ1UVVPD6hXxFgRRJ.png) ![image.png](//image.easyeda.com/pullimage/rAtKJ8SG60uSqeps5NOiVBAw24MTmTllBhDRLKYd.png) This is a vertical mount pot that sits on the top layer of the PCB with the pins pushed in from the top. So to put it on the bottom, place it on the top then swap it onto the bottom. It does not mount with the shaft through the PCB: there is no hole for it. The little cross and the outline of the mounting lug is to help when designing the front panel through which the pot does mount.
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.