Hmmm. Unfortunately it is not possible to diagnose this issue from your images. Please copy your project - stripping out anything you consider sensitive - and check that it exhibits the same behaviour then post the link to it as a public project which to demonstrate this issue by carefully following the procedure described in: [https://easyeda.com/forum/topic/How-to-make-a-Project-public-and-share-the-links-to-it-9f006513b84b412580910905b0281d20](https://easyeda.com/forum/topic/How-to-make-a-Project-public-and-share-the-links-to-it-9f006513b84b412580910905b0281d20)

Right-o.  Here's the link to the project editor page: [https://easyeda\.com/editor\#id=\|8657eeada1934635bf02852fb0e72955\|decba1ca2d4546aa83b325491be1d065](https://easyeda.com/editor#id=|8657eeada1934635bf02852fb0e72955|decba1ca2d4546aa83b325491be1d065)<br> <br>

@billygoat, Thanks for the public project. From that I can see that: 1. In your existing PCB which shows the incorrect Ratlines\, there is a netname mismatch between RB1\_2 and U1\_1\, it is the routing around these nets which is causing the incorrect connectivity and hence Ratlines to appear; 2. If in your existing PCB which shows the incorrect Ratlines, you do **Import Changes...** then the dialogue says that there are no differences between the schematic and the PCB which is clearly not correct; 3. If in your existing PCB which shows the incorrect Ratlines, you do **Edit > Global Delete > Tracks** and then run the Autorouter, the PCB completely and correctly routes; 4. The schematic is constructed correctly and there are no problems when the Schematic Design Manager is run; 5. The schematic converts to PCB with no problems; 6. If after doing **Convert to PCB...** to create a new PCB, the Ratlines in the new PCB are correct to the schematic connectivity and therefore can be routed correctly; 7. What I do not understand is how the tracks came to be routed as they are in your existing PCB, with yourCanvas Routing choices set as they are (Block)  which results in the incorrect connectivity and therefore Ratlines and why they are not corrected when **Import Changes...** is performed. **@UserSupport,** Can you look at the public project to see if you can understand what may have happened to cause the netname mismatch in the PCB? I cannot see how the routing could have been made with the Canvas Routing choices set as they are (Block) and without the Realtime DRC showing errors.

Ah yes\, if I rename the net on the RB1\_2 traces to U1\_1\, then the ratlines come right\. This workaround is enough to make me happy\.  Thanks Andy\!  Happy to work with UserSupport if they'd like to research the problem further\.

Hi Does it correct now, don't understand this problem can you modify this design to simple and indicate which part incorrect?

FYI, I have the same issue, I have added a few new parts and moved somethings around and even on a transfer or import the ratlines remain incorrect.  I think it is something to do with the routes even if partially deleted so they are connected only at one end, retain their old net name, even if the pad they terminate at is on a different net.  Other software dictates the track net to be what ever the pad is it is connected to. If I manually change the track net to match the pad the problem is fixed but it is time consuming and very manual checking between the schematic.  This image shows a mix of pad nets and track nets all mixed up with ratlines still being present and to unrelated nets.  (ignore the track that looks out of place underneath)