2
\$\begingroup\$

I have 53 DIO lines in my circuit. I am designing a multisheet schematic in eagle, and i was thinking about using the "supply" connections as I typically do to connect my supply lines, and a different "supply" symbol with the value and name of the DIO line to connect my DIO pins. However when I do this eagle gives me the error "SUPPLY pin DGND overwritten with more than one signal(LINE1, LINE2, LINE3...etc)."

I know that I can create a wire, and just name it the name of the segment that I want it to connect to, but I don't want a bunch of loose wires seemingly floating around my schematic. What are some techniques that I might use to clean up my schematic and make it professional looking?

\$\endgroup\$
2
\$\begingroup\$

The DGND and other supply symbols connect everything to which they're connected to the same net. This is helpful with common stuff like ground and power, but it's confusing for other nets. Furthermore, you'd need 53 separate symbols for each of your DIO nets, which would not be readable.

Instead, you should use named nets and labels for this purpose.

Issue a name at the command prompt and click a net. A box will pop up prompting you for a new name, enter 'DIO17' or something of that sort. Hit enter, and the net is now named DIO17.

Next, issue label at the command prompt and click a net. The letters "DIO17" are now attached to your cursor. Hit alt to invoke the fine grid, and position the text a few pixels above the net near the end of the line segment.

Finally, do the same for the corresponding net on the other sheet. It will ask you if you want to "Connect N$1 and DIO17?". Hit enter, label the net, and you now have connected these two nets on separate sheets with a readable reference between two sheets. It should look something like this:

screenshot of result

except, of course, the nets will be on separate sheets. If you enter show and click the net, both instances will be highlighted, indicating that the connection has been made.

If you're really insistent that this sort of text label isn't sufficient, and you want symbols, you might consider using the V<-- and V--> symbols in the Supply2 library. These parts won't implicitly connect all the nets attached to them, like DGND and other power symbols. Change their value (ignoring the "Part 'SUPPLY1' has no user definable value. Do you want to change it anyway?" warning) to your net name, and make extra sure to remember to change the net name, and you'll get something like this:

enter image description here

Note that:

  1. That the presence of this symbol with identical text in two places doesn't actually cause these nets to be connected! This is bad.
  2. That this symbol has no pin, otherwise it would need a footprint pad. This may cause trouble when you try to move stuff around.
\$\endgroup\$
  • \$\begingroup\$ As a note, I had to change the eagle schematic for the --> and <-- so that there was a pin to connect to. \$\endgroup\$ – Reid Mar 24 '12 at 22:06
  • \$\begingroup\$ @Reid - I don't think you want to do that, then you'll need an associated pad on your PCB or the footprint won't pass DRC. \$\endgroup\$ – Kevin Vermeer Mar 25 '12 at 1:00
  • \$\begingroup\$ Yeah you are correct, it did not work. Oh well at least your previous answer works well. Thanks! \$\endgroup\$ – Reid Mar 25 '12 at 13:19
1
\$\begingroup\$

First, you should always make explicit power and ground connections. I know Eagle makes implicit connections for you in some cases, but that is dangerous and relying on that feature is really irresponsible.

Second, what you want is called a "bus" in Eagle. It's a way of grouping a bunch of nets together into what is drawn as one fat line. This is useful for showing things like address and data busses. Do HELP BUS and it will tell you all about this.

\$\endgroup\$
  • \$\begingroup\$ Thank you for the help, but the bus command does not do what I need (a symbol for connecting nets), and Unfortunately with a multisheet schematic it is impossible to make explicit supply connections, but on a sheet all supply connections are made explicitly. \$\endgroup\$ – Reid Mar 24 '12 at 20:13
  • \$\begingroup\$ If busses aren't what you want, then you need to describe the problem better. No, you can and should explicitly make all supply connections, whether the schematic uses multiple sheets or not. I have done many multi-sheet Eagle schematics and have NEVER used implicit supply connections. \$\endgroup\$ – Olin Lathrop Mar 24 '12 at 20:38
  • \$\begingroup\$ I appologise for the confusion. I still can't figgure out how to do explicit connections between sheets. Could you please explain how? \$\endgroup\$ – Reid Mar 25 '12 at 13:32

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.