How does the `Connect Pad to Pad` tool work?
4975 5
andyfierman 3 years ago
We strongly recommend that any PCB, no matter how simple, should start as a properly constructed Schematic, with all the correct named nets Schematic Symbols with the correct BOM information and, crucially, PCB Footprints assigned to them, connected by named nets, which is then converted to a PCB. This will save a great deal of work and hugely reduce the chances of mistakes when it comes to checking and submitting the PCB for manufacture. It is, however, possible to create a PCB directly in the PCB Editor, without first creating a Schematic but there are some rules that should be followed to successfully create a PCB this way. If you try to create a PCB in EasyEDA by simply drawing tracks between pads and other tracks then although it may look OK, it will end up generating a very long a list of DRC errors in the Design Manager. This will make it almost impossible to check that the layout is correct. To do this properly, for each individual connected net, all tracks and the pads connected by that net should have the **same** netname. This netname can be the the one that EasyEDA automatically assigns as each element is added to the layout or it can be user assigned but the point is that _everything connected by a particular net_ _**must**_ _have the_ _**same**_ _netname_. This is how the Design Manager understands how tracks and pads are connected together. When following the recommended Design Flow in EasyEDA, all this work is done in the creation of the Schematic so that, on doing **Convert to PCB...**, all the connectivity, netnames and the correct library PCB Footprints are passed straight into the PCB Editor so that PCB layout can start immediately. When creating a PCB without a Schematic, this work of identifying the connectivity and naming the tracks and pads has to be done manually. This can be done entirely manually by editing every track and pad as, or after, they are laid down but it is much easier to do this using the **Connect-Pad-To-Pad** tool. However, it is important to understand how to use this tool. * The **Connect Pad to Pad** tool will _not_ draw ratlines between isolated pads or vias that are not part of a component PCB footprint. * The **Connect Pad to Pad** tool in the **PCB Tools** palette is to draw ratlines between the pads of PCB footprints, even if the footprints are on different sides of the PCB. This tool is used to build a netlist of the connectivity of a PCB that is being created without a schematic. (However, please see: https://easyeda\.com/forum/topic/The\_best\_way\_to\_design\_a\_PCB\_in\_EasyEDA\-ThR3pwqIC for an explanation of why it is much better to create a schematic first and then convert that to a PCB.) If you place some PCB footprints on a new PCB and then use the **Connect Pad to Pad** tool, you will find that EasyEDA draws the ratlines. The **Connect Pad to Pad** tool does not work just connecting isolated pads or vias, because they are physical elements of the routing between the pads on components and so are layout dependent. For example if there are two SMD footprints both on the same side of the board then no vias would be needed to connect the pads but if the two components are on opposite sides of the board then vias would be needed to complete the routing between the component pads. This means that the isolated pads or vias are not directly part of the connectivity between a pair of component pads and so are not something you can draw a ratline to or from. If you need to place a single pad somewhere then you can use a single pin through hole PCB footprint such as HDR1X1 (from the EasyEDA Libs) or a surface mount single pad PCB footprint such as Test_Point from the SHIFT+F searchable library. Once the basic PCB design has been connected up using the **Connect Pad to Pad** tool then routing (tracking) can be started with any vias needed to change layers placed as required as routing progresses. For more information about Ratlines, please see: [https://easyeda.com/forum/topic/Understanding-Ratlines-371bdbf646c54b23a57451eb05b2026d](https://easyeda.com/forum/topic/Understanding-Ratlines-371bdbf646c54b23a57451eb05b2026d)
Comments
susmanhaider 1 year ago
how to undo connect pad to pad
Reply
andyfierman 1 year ago
1. Select all the pads that you want to remove the connections between (Hold CTRL + Left-click on each pad in turn); 2. In the right hand panel find the `Net` attribute; 3. Delete the text in the `Net` attribute field.
Reply
andyfierman 1 year ago
1. Select all the pads that you want to remove the connections between (Hold CTRL + Left-click on each pad in turn); 2. In the right hand panel find the `Net` attribute; 3. Delete the text in the `Net` attribute field.
Reply
daliborovcin 1 month ago
@andyfierman Please make video tutorial...this is so frustrating!
Reply
andyfierman 4 weeks ago
@daliborovcin, Please read: [https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a](https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a) and post your question clearly in a new thread.
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.