Printing Double Sided PCB and Creating Silk Screen from Laser Printer Toner

My recent project, an ATTINY84 with an ICSP header, could not have all of its traces on a single side of copper. In the past when I have had this problem, I have simply run a wire or two across the top to solve the problem. I decided it was time to do it right and produce a double sided PCB.

After going thru the exercise once, I realized it was trivial to add toner printing to the top of the board like silk screen. So I decided to do the process again creating 2 sides of copper and then placing a toner layer of text and images (silk screen) on top of the copper.

I kept notes of this process, and I’m recording them here primarily for my own use, but someone else might find the process useful. As such, I omit certain big things such as how to do toner transfer and etch the board. This procedure is mainly about getting the various layers properly registered (aligned).

Create the Schematic

  • I use Eagle Cad to design my circuit and layout the PCB. My examples will be from it. Here is the schematic for this simple circuit:


Layout the PCB

  • Eagle appears to have updated their hole symbol. See April 2015 Update at the bottom as to how I handle this.
  • Start by selecting the hole tool.  I use a .3″ hole to create register marks. These holes are what you will use to align the top and bottom layers. You only need two holes.
  • I place one hole in a corner and then I place the other half way up the other side. This non-symmetrical hole alignment keeps me from screwing up the direction of the images when I place them on the front and back of the board (my first board had holes at opposite corners and sure enough I got the top and the bottom layers reversed. Argh!)


  • Layout the PCB as you wish.

Auto-route the Bottom Traces

  • Go to Edit | Net Classes. I set default width/drill/clearance to 30/20/30mils. I’ve had trouble in the past with traces smaller than this.
  • Create a solid fill polygon on the bottom layer of the board and name this polygon GND. I like to leave a nice margin around the components and the edge of the polygon so autorouting has more room if it needs it. Once routing is done, I can move the polygon in tighter.
  • Click on Rats Nest to fill in the polygon.
  • Click on the router button. For top I use N/A. For the bottom I use * or Auto (both seem to be about the same to me). For effort I use high. Even though this procedure is about creating a double sided board, I want as few traces on the top as possible which is why I set top to N/A.
  • Let the auto-router do its thing, and select the route you like best.
  • After routing is done, check the lower left corner, and it will tell you how many air-wires are left. If there are any left, you will need a top layer.


  • Locate the air-wire on the board layout:


Tying Ground Islands Together on the Top Layer

  • Since we are not using auto-routing to create top traces, and we have a ground polygon, the most common reason, from what I’ve seen, for air-wires to remain after auto-routing, is due to ground islands.
  • Ground Islands are parts of the board that are no longer grounded because other traces cut the island off from the rest of the ground plane.
  • If you look at the figure below, the white arrow points to the ground plane polygon. The red arrow points to a ground island that is isolated from the rest of the ground plane:


  • We just need to connect the ground island to the rest of the ground plane and the air-wire will go away. To do this, we will put vias on both the ground plane and the ground island. Then the two are connected together with a trace on the top layer of the board.
  • Select the Via tool, and set it up. I suggest setting the diameter fairly large. That way if the top and bottom layers’ alignment are off just a little, you will have some leeway with the hole that connects the top to the bottom.


  • Place the vias somewhere in the ground island and somewhere in the ground plane:


  • Name each via GND. Click on rats nest. The air-wire might move to the via (it did for me). No problem if it didn’t.
  • Select the wire tool and set it up. Look at the property of an existing trace to determine the width. Make sure you are on the top layer (the trace will be red):


  • Draw a wire between the two vias. Then right click | properties for the wire and verify it is named GND.


  • Click Rats Nest. Once all ground islands are tied together there should be no air-wires left.

Connecting Component Legs with Top Layer Traces

  • With my first attempt at a double sided PCB, I let auto-routing create traces on the top and bottom of the board.
  • I, incorrectly, thought if I just soldered the bottom of the component leg the solder would flow down and magically adhere to the pad on the top of the board. Wrong!
  • It was difficult to solder components to the top of the board. This was particularly true of IC sockets and header pins. I managed to solder them, but the board was very messy.
  • Instead, if you need to run a trace on the top layer between two components, you need to create vias in front of each component leg. Run a trace on the bottom layer from the component legs’ to their corresponding vias. Then run a trace on the top of the board between the vias.
  • In the figure below, the circled areas show where I put a via in front of each leg that needed to be routed on the top of the board.
  • While this works, it makes the layout more difficult to design and solder, so I just try to minimize the top traces as much as possible.


Make the Board Look Nice

  • I like to place the board name and revision on the bottom of the board in copper. Use the text tool and make sure the bottom layer is selected.
  • When you initially place the text on the board, it will disappear. This is because it blends in with the blue polygon. Click on Rats Nest and it will appear properly.
  • You can do the same for the top layer since you are doing a double sided board. What you use here depends on if you will also do a toner silk screen layer.
  • From my initial experiences, using copper for art-work and text is good if the text is somewhat larger and no danger of coming in contact with any signals on that layer. Toner silk screen may wear off a little easier, but it can produce finer lines and is non-conductive.
  • If you are going to print the toner silk screen layer, fix that layer to look nice. You can smash the components and then rotate and move the text as necessary. To see just the toner silk screen layers, turn off just layers 1, 16, 17, and 18. You can add new text to layer 25 for the toner silk screen.
  • Here is the Board ready to be printed:


  • My last step before printing is to convert the solid polygon to a hatched polygon. When I etch large solid copper, it never looks great. This seems to help a bit.

Export to Photoshop for Final Touches

  • I use Photoshop for the final touch ups. You can also use GIMP or just print to your laser printer directly. My examples are using Photoshop.
  • Eagle Cad will only print each layer one at a time. While you can mess around and print multiple times on each page until you get all three layers, I find it just as easy to export all three images to Photoshop and combine them into a single page there. Using Photoshop also allows for insertion of any art-work.
  • Print Bottom Layer
    • Select Layers 16, 17, 18, & 45
    • File | Print and select Print to File (PDF) – found at very bottom of drop down box.
    • Options: select Black.
  • Print Top Layer
    • Select Layers 1, 18, 45
    • File | Print and select Print to File (PDF)
    • Options: select Black and Mirror.
  • Print tone silk screen Layer
    • Select all layers, then unselect layers 1, 16, 17, 18, 19, 20
    • File | Print and select Print to File (PDF)
    • Options: select Black and Mirror.
  • Open the PDF files you just created in Photoshop.
  • When importing the PDF into Photoshop, use resolution of 12oo pixels/inch.
  • Open a new document makeit roughly 8×10″ and 1200 pixels/inch (must match resolution used in prior step).


  • If you want to create art work on any of the layers, this is the place to do it. The artwork must be only black and white (the black will contain copper and the white will have it etched away).
  • Don’t forget to flip the artwork on the horizontal axis so it will be oriented correctly after the etching process.
  • I inserted this little thunderbolt on my board as an example of what can be done.
  • CHECK that any additional art-work will not conflict with the other layers. I didn’t do that and sure enough the tip of the lightning bolt was on top of a via.
  • In the future I will look at putting a box in the board design where I want the graphic. Then I can see any possible conflicts there and make sure the graphic fits into the box once I’m in Photoshop.


  • Copy all three images into the empty page sized doc and align them as you wish so they all print on a single sheet:


  • At this point, I print this on a normal sheet of paper, cut out the 3 layers, hold them up to the light and align the holes to verify everything looks reasonable.
  • Now print the image on the toner paper of your choice. Cut the 3 layers into individual pieces.

Register/Align the Toner Images on the PCB

  • Insert a push pin thru the center of each hole for all three images. You need to be as precise as possible. The drill holes in the vias are .03″ – there is not much room for error. I have found if I have a bright light near the paper, I can watch the pin and its shadow to more precisely hit the very center.


  • Using heat proof Kapton tape, tape the bottom layer image to the PCB.
  • Drill a hole thru the hole in the paper and through the PCB. I use a .05″ drill bit for this which is just barely larger than the thumb tack I will be using.
  • Remove the tape. Using compressed air, blow the drilling residue off of the PCB and the paper. I didn’t do this on my first attempt and the dust prevented the toner transfer from working cleanly.
  • Use thumb tacks to realign the bottom layer to the PCB and tape into place:


  • Flip the board over and tape the top layer paper face down over the tacks and tape to the board (the toner silk screen layer will be used after etching is completed).
  • With both sides taped, you can now remove the thumb tacks.
  • Transfer the toner with heat and and etch the board (these procedures are beyond the scope of this document).

Applying the Toner Silk Screen

You can probably guess the rest! Once the board has been etched and tinned, you are ready to apply the toner silk screen.

  • Align the toner silk screen image onto the top of the board using thumb tacks and tape into place.
  • Transfer the toner with heat and clean the paper from the board.

Here is the top of my bare PCB:


Looks pretty nice except for the aforementioned artwork over lapping a trace. Ugh!

And finally, the populated board:


I’m really happy with the overall quality of the board. Not at all bad for home brew!

April 2015 Update:

I’m laying out a board today and the hole tool no longer has a cross hair thru the center, just a single slash. I really liked that cross hair as it help me get the needle aligned right in the center.

There are some holes in the library that have crosses, but they are gigantic so I don’t want to use them. The best alternative I’ve found is to create a pad with the following properties:


When I print this it ends up producing a circle with cross hairs in it.


This entry was posted in c-electronics and tagged . Bookmark the permalink.

Leave a Reply

Fill in your details below or click an icon to log in: Logo

You are commenting using your account. Log Out / Change )

Twitter picture

You are commenting using your Twitter account. Log Out / Change )

Facebook photo

You are commenting using your Facebook account. Log Out / Change )

Google+ photo

You are commenting using your Google+ account. Log Out / Change )

Connecting to %s