I'd like to create arrows in my schematic. The solution (using XREF) to an older, related post gets me most of the way there:

Arrows on connections in schematics

BUT, with that approach, the net always connects to the pointy part of the label symbol, effectively making all labels look like inputs. Mirroring the label, or rotating it 180 degrees does not solve this problem. Does anybody have a work-around? e.g. is it possible to make a set of devices (INPUT, OUTPUT, INOUT, etc.) that have symbols and a pin to tie to a net, but no associated packages?

Here is an example of what I'd like to have:

enter image description here

And here is what I can do in EAGLE so far (notice that my OUTPUT is a mirrored version of the input, but the net is drawn through the label in order to connect to the vertex. What I'd like is for the net to connect to flat side of the output label (i.e. on the left side of the label, near the letter "O" in the example below, and as in the CE, CSN, MOSI and SCK labels in the image above).

enter image description here


Just drag the output label over. It doesn't need to be touching the net at the label origin.

enter image description here

Note: To remove those little origin markers, use the set Option.ShowTextOrigins 0; command. Also note that this does not disconnect the label from the net, they are still associated (renaming the net will change the label). This simply moves the origin to not be on top of the net, so the two must be selected with the selection tool before being moved.

  • \$\begingroup\$ I don't think this is a full solution for the following reasons: (1) no guarantee that the net will actually touch the label since only the pointy front is on the 0.1" grid (looks like you have a very fine grid in your screen grab). (2) The label is not actually electrically connected to the net. But is it possible to make a device that has the anchor point on the flat edge (and has no associated package)? \$\endgroup\$ – James Jul 27 '15 at 19:05
  • \$\begingroup\$ @James (1) Make your grid smaller, adjust the label, then reset your grid. The label will move with the net in grid increments. (2) The label is connected to the net. If you grab and move the label you will see a little white line connected right onto the end of the net. (3) You can't create a symbol with a pin and no package. (4) You asked for a work-around, what sort of "full solution" were you looking for instead? \$\endgroup\$ – Samuel Jul 27 '15 at 19:11
  • \$\begingroup\$ I take back my (2) -- you're right, the label is connected to the net. I tried your suggestion a bit and find it easy to do (I leave the grid spacing at 0.1" but place label with the Alt pressed, no grid snap). The only downside that I see at this point is that if you move the label, the net does not follow (unless the net is connected to the origin at the pointy end of the label). re: full soln, I've used other schematic capture software (gschem, Altium), and they had ways to mark "net stubs" (if I remember the name correctly) as inputs or outputs, and net would travel with stub. \$\endgroup\$ – James Jul 27 '15 at 19:28
  • \$\begingroup\$ @James The alt does have grid snap, it's just default set to a much smaller grid (default 10 mil). The label does not move with the net if you select it alone, but if you use the selection tool and select both the very end of the net and the point of the label and do a 'move group' it will move just like it was attached on the flat edge. \$\endgroup\$ – Samuel Jul 27 '15 at 19:36
  • \$\begingroup\$ thank you for the helpful explanations. As you point out, I did ask for a work-around, and this is a good one, so I'll accept your answer. If you have ideas of how to set the anchor point to the flat edge, or how to have an INOUT shape (points on both sides of the label), I'd be interested to hear about them. \$\endgroup\$ – James Jul 27 '15 at 19:40

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.