EAGLE: how to find where the pin is connected - navigating fairly large schematics

Question

I have a fairly large schematic loaded in EAGLE (netlist file is ~2500 lines long) and I want to find out where exactly some pin is connected, given chip name and pin name.

What I'm trying to do:

• I can easily locate chip in question on the zoomed out view, it's not too many of them and they're clearly labelled
• I can more or less quickly locate desired pin by browsing through all the pins of the chip (it's "less quickly" if the chip in question is a CPU with ~600 pins)
• I can trace where the wire goes then by eye, but there are two major obstacles: buses and named nets. Both basically mean that this point connects to the net that can be scattered all around the drawing.

What I already tried:

• "Info" command makes it possible to highlight only one particular instance of the net/bus connected, not highlighting all the rest.
• "Show" command technically does exactly what I want - it highlights all the connected pieces in all instances of the net, but this highlighting stuff is fairly hard to notice (contrast between "highlighted" and "normal" is not so great) and basically it only works on high zoom levels (where there's at most 8-10 inches fit on the screen). Hunting for that "highlighted" pixels on bird's eye view is very tedious task.
• find.ulp can highlight and zoom onto particular element by name, and that works for nets too. But, alas, I can't seem to understand how it works:
  • Just asking for net/bus by name (with count=0 by default) yields random piece of that net
  • Asking for net/bus by name + count=1000 yields another pretty much random piece of that net, and reports how much of them are available (for example, "9")
  • Then asking for net/bus name + count=(1..9) tends to yield various pieces of the net, but sometimes they clearly repeat and the result seems to be pretty much random. How can I make sure that I've browsed through all 9 instances of a given net?

Any tips on how seasoned pros get through this basic navigation stuff? I might guess there's a way to add more contrast to highlighting to make it more obvious, or there's some proper way to use find.ulp to iterate over every one of the pieces of the net/bus?

Answer 1

As others mentioned in the comments, a best way to deal with large schematics is to avoid large schematics, by splitting them into many smaller sheets.

As to find.ulp, you are using it just right. What you must understand is that, every net segment is treated separately, so if you have something like:

    |
    |
____._____

find will yield three results for it. That is probably why you have an impression that results repeat. Anyway, you can browse through all of the results by typing RUN find NAME nand increasing n by 1. Theoretically, RUN find NAME + should let you browse through all of the results, but for me it works only in board view, not in the schematic.

Also, try typing SHOW @ NAME, it will draw a rectangle around all highlighted elements, to locate them more easily.

Answer 2

Type Show @ US0_* for example, and Eagle will either:

1. If references are all on one sheet: Highlight all matched nets and draw a box around the area containing the references, or

2. If references are on multiple sheets: pop up a dialog listing a references, where you can click on each list entry to bring up the appropriate sheet and highlight the specific reference

Hope that helps someone out there.