Home>Forum>Topic
Latest Topics Latest Replies EasyEDA Std EasyEDA Pro JLCPCB LCSC OSHWLAB General Discuss
Schematic PCB Simulation Skill Extension Feature Requests Bug Reports
You need to use EasyEDA editor to create some projects before publishing
Wrong Ratlines are shown in PCB Layout (Project: CNC Controller)
471 12
PhilippEBZ 3 years ago
Hi, I've got a problem with routing the PCB. This is my first layout with EasyEDA, I have not much layouting experience, I did one PCB with EAGLE in uni years ago, so please be gentle, I might do something wrong, but I am here to learn :) My first project might be a little to much to, is not the simplest thing, but I am motivated and hoping to get through. I'm trying to make a CNC controller on basis of the following project: [https://github.com/bdring/Grbl_Esp32](https://github.com/bdring/Grbl_Esp32)                         (Software) [https://github\.com/bdring/6\-Pack\_CNC\_Controller](https://github.com/bdring/6-Pack_CNC_Controller)    (Hardware) So I made the circuit according to my liking with all the features and connections I need, and everything worked fine. Next I created a PCB and started to play around there, made a couple attempts, acutally :D... Anyway, I also played arround with the Auto Router and then I noticed that something in the PCB is not according to the circuit. I updated and imported changes etc, but I keeps showing me wrong connections. <br> Here on JP2 you can see that Pin 9 is supposed to be the Enable for Stepper 6 (Stpr_6_En). ![image.png](//image.easyeda.com/pullimage/YSaUTGK5ofgnBFWsjT8fxuzTM5kktmlwlyuTvX9h.png) But in the PCB at the bottom (marked white) you can see that the AutoRouter connected that pin with a couple of others and it thinks it is the Alarm of Stepper 2: ![2021-03-21 17_52_41-EasyEDA(Standard) - A Simple and Powerful Electronic Circuit Design Tool.png](//image.easyeda.com/pullimage/Wq8tkMuAaJDOZt5TLwWgQVaSZZJk1QkNgj7UdPa0.png) ![image.png](//image.easyeda.com/pullimage/9rfIZ1QzWWlyb0MNuVioVPH41tqKnKMFK3mLK7zI.png) I tried to make the project public, so i guess anyone could access: [https://oshwlab.com/PhilippEBZ/6axis_pk](https://oshwlab.com/PhilippEBZ/6axis_pk)<br> <br> The circuit screenshot is in 1_outputs and the pcb screenshots are from the PCB file called PCB\_AutoRouter\_2021\-03\-19 <br> Please enlighten me, what I am doing wrong!? Greetings, Philipp <br> <br>
Comments
MrToM 3 years ago
If you ckick on the Net Port 'Stpr\_6\_En' you'll see in the right hand panel that its actually the Net Port 'Stpr\_2\_Alarm'\.\.\.\.so the autorouter was correct\. Just to be clear, when I say 'Click on the Net Port' I mean the actual port, the 'rectangular arrow' shaped lable....not the text next to it. _ What you've done, and totally understandably too, is to edit the Net Ports name, (the text associated with it), but not the actual Net Port itself. Yeah\, I know\.\.\.\.confusing but it's an easy fix\.\.\.\.just make sure the Net Name IS the name of the Net\.\.\.\.ie 'Stpr\_6\_En' and not 'Stpr\_2\_Alarm'\. _ Regards.
Reply
andyfierman 3 years ago
I think there is something else going on here. It does not matter if you edit the name of the NETFLAG in the schematic or in the right hand panel: the two operations are exactly equivalent. In the following, C9, C21 and the BOO netflag are my additions to try something out. Refresh the nets; Click on the BOO net in the Design Manager: ![image.png](//image.easyeda.com/pullimage/YIC1XLAiahhVbLaQfYlXQXmJ0O5h8BIlznJI98Ub.png) The BOO net is correctly reported _and the pins connected to it._ Remove C21, refresh the nets then click on the BOO net again: ![image.png](//image.easyeda.com/pullimage/UpKdNL1SBcyYvD7I9RDGSf8zODkXnrmUBYtbVdIV.png) The BOO net is correctly reported _and the pins connected to it._ Then... Tried the same thing again and this time got: ![image.png](//image.easyeda.com/pullimage/ADjfpOvdYxXpIFZ2CFO03dr4E4IW7CqAMV7P4AlO.png) No pins report and no incomplete net warning! Getting the same behaviour on Stpr_6_EN it lights up but no pins or incomplete net warning message. It lights up on U16 but not on J2: ![image.png](//image.easyeda.com/pullimage/FVvVhI0hgGNlYLL8WCkLuNMHA23M2zkyWd5YeB1w.png) Click on Stpr\_2\_Alarm then Stpr\_2\_Alarm **and** Stpr_4_Alarm on J1 **and** Stpr_6_En on J2 light up but no pin information: Stpr_2_Alarm ![image.png](//image.easyeda.com/pullimage/l3bl8FBu9tiJLw6L1e2g4aKetBpn59UULHOPJtvZ.png) but the Design Manager is not warning about other different net labels being applied to the same net! **I don't have time to look into this more right now but I suggest that you change the Category of this post to Bug Report and freeze this project or clone it to preserve the status until @UserSupport can have a look at it.**
Reply
MrToM 3 years ago
Just to clarify... The wrong NET name... ![01.png](//image.easyeda.com/pullimage/gOHrwiQWFaEZPM3N5J6sUu2vM9d9NqHnj4D9c4Y8.png) _ Enter the right NET name... ![02.png](//image.easyeda.com/pullimage/OFDIfTij0I9P2ME49mN76I5WCla2E4AuiYB7Mka0.png) _ ...and this... ![03.png](//image.easyeda.com/pullimage/IXxyOtQgkVZMmQaczwvC3qfgRih6XoGVgsyRaa8Y.png) _ ...when updated... ![04.png](//image.easyeda.com/pullimage/c7w4tfd8kFCYE58sPZ7ffLk9Hrlc1xvZdb6dTi23.png) _ ...results in the correct ratlines... ![05.png](//image.easyeda.com/pullimage/eeh9gDrgESqUAzXigBuU2Bb025G5tGtiWJ8NCKGp.png) _ Which is how I read the OP's question...rightly or wrongly. _ Regards.
Reply
andyfierman 3 years ago
@mrtom528, Yes, you are absolutely correct and your solution corrects the mis-naming that the OP was asking about. In my screenshots etc. above, I missed commenting on the fact that the Stpr_6_En label and name were different depending on whether you clicked on the text or the symbol. **However**: There is a much more worrying issue here. The mismatch between the name of the netflag shown in the text in the schematic and the name shown in the right hand panel when you click on the symbol for the netflag should not happen! Whenever I enter a netflag, if I edit the name on the schematic or if I click on the symbol and edit the name in the right hand panel: they end up being the same. I cannot create a different name on the schematic from that shown in the right hand panel no matter how I edit the name. * So the first question is: how did this come about in the OP's project? It is not just the Stpr\_6\_En net that needs to be corrected\, Stpr\_4\_Alarm flag is wrong too: ![image.png](//image.easyeda.com/pullimage/9Wc3nLwW2aLRFvQRa8MWm3l4jK92P5O4ltgRhy5J.png) * The second question is: why does the clicking on a net in the Design Manager produce the two differnt responses as shown in my post regarding the BOO net? * And a third question is: what has gone wrong with the net to pin connection identification in the OP's project, in comparison with my added BOO net and connections to C9 and C21, also as shown in my screenshots? <br> <br>
Reply
MrToM 3 years ago
@andyfierman, Ah...sorry, I hadn't read your post before starting the lengthy construction of mine...which was purely aimed at the OP to clarify my scribblings. _ I fullty understand your thinking here but what about this... _ 1\. COPY the Net Port 2\. PASTE the Net Port 3\. Change the TEXT\.\.\.\.\.and completely forget to change the NET Name in the right hand panel\.\.\.??? _ I know I've done it before....many times. Could it just be a simple PEBCAK? _ Regards.
Reply
MrToM 3 years ago
@mrtom528, Ah-ha! _ I see where I'm going wwrong.........not enough G+T's! _ I get ya now......It looks as if the OP has turned off displaying then name, added some text to compensate and just didn't realise that it didn't link....I think, ya see? I should have noticed that the lable AND the text should have highlighted but didn't as I can see twoo of everything. Sorry for my slappiness. _ I need a dringk. _ Regrads.
Reply
andyfierman 3 years ago
@mrtom528, Aaaaaaaargh! Yes, that's it. I didn't spot: **Display Name = No** in the right hand panel. Turning the Display Name back on and correcting the names should then sort out the connectivity.
Reply
MrToM 3 years ago
@andyfierman, Aaaaaaaargh! Indeed! _ Harumph. _ Regards.
Reply
andyfierman 3 years ago
@PhilippEBZ, Please set the visibility of all your netflags to Yes then correct the netnames as required and then delete the spurious text. You can select all the netflags at once by selecting one and then using Find Similar Objects... set to All Sheets: ![image.png](//image.easyeda.com/pullimage/KFIjVNqcoGNZUfqobZ2EzuiP8GfCq4FqIZBTcQRd.png) After you have done that please let us know so we can check out the other issues with net to pin identification. Thanks.
Reply
PhilippEBZ 3 years ago
Hey guys! Thank you so much for that amazing analysation! I hoped it to be a case like this, where copy pasting or renaming screwed it up! I will correct that and let you know if everything works for me! Thank you, have a good day
Reply
fbrier 1 year ago
@andyfierman This was a helpful post. I had an almost identical problem/error message because I did not assign Net names to some of the pins on a Raspberry Pi GPIO 40 pin connector. The auto-router was tying them together. By adding a Net symbol to the wiring connection, it resolved the errors.
Reply
andyfierman 1 year ago
@fbrier, Thank you. It's nice to know that at least some of my replies can be found by the search tools and are helpful. :)
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