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.




    • PCB Contest

      PCB Contest
    • Epilog X Contest

      Epilog X Contest
    • Safe and Secure Challenge

      Safe and Secure Challenge

    9 Discussions


    3 years ago on Introduction

    I pick NA (Not Applicable/Available) for the top layer, and * for the bottom, when I auto route. The top layer is eliminated then.

    4 replies

    Reply 3 years ago on Introduction

    As such, that's how you'd aim for a single-sided PCB layout. But it won't necessarily result in a fully routed design. If there are traces that NEED to cross and can't be routed using only the bottom layer you'll be left with a number of airwires.

    Of course, there are several ways to solve that. Maybe you can rearrange the parts, use different ones, or give in and put in jumper wires. But the point of this Instructable was basically to show how to modify existing library parts to help solve a placement problem.


    Reply 3 years ago on Introduction

    It is rare that I cannot route a board 100%. I tend to stick with simple designs. I don't etch boards anyways, so every wire I use is a jumper. Here's the one I made yesterday


    Piece of cake. I only thought one wire even needed insulation, as the rest are far enough from each other, they cannot short out. Here is the board layout for that


    I print that on plain paper, then tape it to the plain board I build my circuits on. I use the print out as a drill guide. Here's the top


    It looks like any other circuit board. So skip etching.


    Reply 3 years ago on Introduction

    Sure, I've made boards like that, and also by milling the isolation tracks in a copper-clad board with a Dremel (even double-sided in one case). But once you get into somewhat more complex boards I think you'd prefer etching, which is where this Instructable is aimed at.


    Reply 3 years ago on Introduction

    Even though I only wire boards up point to point I still want my designs routed on the bottom layer. Etching is messy with the chemicals. I've done it.



    Instead of etching I've decided I'd rather just get on with it, and build circuits. Etching is handy if you plan on making multiple boards. Which is something I am not interested in doing. I like to make different circuits. Once I've made a circuit I've little interest in making another of it. Believe me, I've thought about all of this a lot.


    3 years ago on Introduction

    Most board houses can go down to 6mil traces, so changing the part would be more work than to change the trace width.

    1 reply

    Reply 3 years ago on Introduction

    If you'd read the lead-in, and the Instructable that it links to, it might have pegged that this is about designing the board so you can etch it yourself.

    Eric Brouwer

    3 years ago on Introduction

    Thanks for the instructables on Eagle. I have been using Eagle for a while now, but after going through this, I know so much more about Eagle.