PCB's: Can I Get Rid of That #^%$! Top Layer Trace?

So, you've designed a circuit, and turned it into a PCB design, following this Instructable. Looks good. Except for that single one irritating top-layer trace. It looks like you could run it between the legs of one of the transistors ... Unfortunately, the design rules that make it easy for you to etch the board yourself: wide traces and matching isolation, block that. Now what?

Okay, it's easy enough to just run a wire where the trace needs to go, but it's not neat. You dislike doing it like that. If you were building on perfboard you could just spread out those transistors' legs ... eureka!

Step 1: The Schematic

So, here's the schematic again. It's drawn differently, but essentially the same as in this Instructable.

As an aside: you may have noticed that my schematic and PCB look roughly mirrored from the one in the link above. I prefer to have inputs (or in this case the signal source) on the left, outputs on the right.

Now, of course this won't work with just any part, but you have probably noticed that the Eagle libraries have through-hole parts like resistors and capacitors in several sizes and pin spacings. Some transistors too, but not the ones used for this schematic. So, we'll have to edit them.

It used to be that creating or editing library parts in Eagle was rather cumbersome. As from version 7, it has gotten quite a bit easier: you select the part you want to modify in the schematic editor or the board editor, right-click and select 'Open Device' or 'Open Package'. In this case, you can choose either, because you actually want the index for the library containing that part.

Step 2: Editing the Part

And here it is, the device. Which shows you that it is a transistor with a TO-39 case. With legs that you could bend, if ...

The library editor in Eagle version 7 has another nice feature: it can show a list of the symbols, packages and devices, by clicking on the icon that looks like a book (fourth from the left in the upper icon bar).

Step 3: Editing the Part, Part 2

The packages are in the middle column.

We're going to duplicate the original TO39, so as not to mess up the footprint of every other device using the TO39 package. Select the package, right-click, choose 'duplicate', then enter the name for the new package. I went for TO39-EW (Extra Wide).

Step 4: Editing the Package

Now you can move the pads outwards, in the screenshot above there's one pad done, two to go.

Of course you can move the pads further out still for an even wider version, but that's just a matter of repeating the previous steps once more to create yet one more copy of the package.

Step 5: Adding the Package to the Device

Now the modified package needs to be tied to the part. Select the device, then press 'New' in the lower right of the window. A new window pops up, from which you can select the TO39-EW you just created.

Step 6: And Connect the Pins to the Pads

As the pinout for the -EW package is identical to the original TO39 package, this is as simple as can be. Use the 'Copy From' drop-down box, select the TO39 entry (the only one in this case) and press OK.

Done. Or rather, nearly done, because there are two transistors in the schematic, from two different libraries: transistor-npn and transistor-pnp. We've just modified one, now to copy the new package to the other.

Step 7: Copying the Package Into the Other Library

Save and close the library you've been editing (transistor-npn), and open transistor-pnp, then go back to the control panel. Expand the transistor-npn library, and the package tree in it. Locate the TO39-EW package you created, then simply right-click and select 'Copy to Library'. Now you can repeat the two previous steps to again add the -EW package to, in this case, the 2N2905. Now we're ready to actually modify the board

Step 8: Replacing the Parts in the Schematic

Again, a rather obvious and straightforward step. Select one of the transistors, click the 'replace' button in the left-hand toolbar (below the 'add' tool), then select the transistor with the newly-created package from the library. You'll see a pop-up message notifying you that the library has been changed, and the part in the schematic (and the board) needs to be updated.

Of course you click 'yes; why else would you have been fiddling with the library editor then?

You can do this from the board too.

Step 9: Not Quite There Yet

The new parts are now on the board. but there's some re-routing to do.

Step 10: Ripup

Pillage! Plunder! Destroy!

Oh, sorry, got carried away. Just ripup. And double-click that #^%$! Top Layer Trace.

Step 11: And Route the Resulting Airwire

As the transistors' legs are now spaced more wide, the trace that Used To Be That #^%$! Top Layer Trace can now stay on the bottom.

Done.