In the past I designed a PCB on EAGLE, and now I want to make some changes on it, but it's impossible. You can see it in the picture below:

Problem picture

In the old schematic part I can move and delete nets, but I can't stick a new line or new elements to an old design part. It looks as if my schematic is separated into the old design and the new design, and I can't connect these two together.

  • \$\begingroup\$ If you ctrl+click on the end of wire, or on an object, it will re-grid that object. \$\endgroup\$ Aug 12, 2015 at 14:00
  • \$\begingroup\$ Alternatively, if you want to do the whole schematic enter the following command: run snap-on-grid-sch \$\endgroup\$ Aug 12, 2015 at 14:02
  • \$\begingroup\$ thank you Mr. @TomCarpenter your answer was what exactly i looked for , thank u very much . \$\endgroup\$
    – user83106
    Aug 12, 2015 at 14:05
  • \$\begingroup\$ Woops, looks like Tom beat me to it. I should have read these comments first :p \$\endgroup\$
    – DerStrom8
    Aug 12, 2015 at 14:06

2 Answers 2


This means that the schematic was designed with a different grid setting that the new one. Even if the grid size was the same it is possible that the origin has moved (if say you selected all and moved the group with the alt grid).

With a schematic, unlike the PCB, really everything should be on a strict grid, it is only Text Labels that should be allowed to be placed off grid (and even then I would still stick to the grid!).

For single wires you can ctrl+click on the end point of the wire to pull it back to the current grid. You can do the same with the origin points of components. However this only works if a very small number of bits are off grid. For a large schematic it would take a very long time to individually re-grid every component.

Fortunately, there is a quick solution to restore the entire schematic if it has ended up off-grid. In the schematic window, enter the following command:

run snap-on-grid-sch

What this will do is set the origin of every component and end points of every wire to be on grid. You can select the grid using that ULP, but I would advise sticking to the default grid of 100mil as most components will be designed that way.

  • \$\begingroup\$ This is a much better approach than mine. \$\endgroup\$
    – DerStrom8
    Aug 12, 2015 at 14:08

The problem is that your grid does not match the grid used to create the original schematic. ctrl+click changes to a much finer grid which will allow you to make the connections. How complicated is the schematic? If it's not too complex, you may want to redraw the entire thing using your own grid.

This often happens when drawing the schematic in a metric grid and opening in an imperial grid, or vice versa. The same goes for PCB routing.


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.