Manufacturing PCB layouts made in KiCad

Up to this point I have made all my printed circuit boards at home, which is great fun and comes with a great sense of satisfaction when your circuit finally works. But it also takes a lot of time, expensive, and you have to deal with messy corrosive chemicals. But if you really like to print your circuit layout at home, check out how I did it here.

But now I am ready to outsource the manufacturing of my PCB layouts. One of my colleagues told me about this awesome community PCB manufacturing site called OSH Park, where you can get your layout printed at a very reasonable price. And they don’t require you to order a massive number of boards.

I finally finished laying out the component footprints and traces for my new and improved Gyro’clock circuit. Before doing this I ordered all the parts so that I can check them for reference while I am creating some of the custom footprints, and also I don’t run the risk of using obsolete parts after I have manufactured the boards. Here is what my finished design (all layers) looks like in KiCad

New and improved Gyro'clock layout in KiCad
New and improved Gyro’clock layout in KiCad

The 2-layer board is 6.2 cm by 2.9 cm. Not the ideal size I wanted, but I like how everything fits nicely. I chose the following design rules before doing the layout as per specifications on the OSH Park website:

  • minimum trace width: 0.1524 mm (6 mil)
  • minimum via diameter: 0.6858 mm (27 mil)

My default net class values used for all the connections are the following:

  • trace width: 0.2032 mm (8 mil)
  • trace clearance: 0.2540 mm (10 mil)
  • via diameter: 0.6858 mm (27 mil)
  • via drill: 0.3302 mm (13 mil)

I placed all the component on the top plane and made the bottom side into a ground plane, but had to route some traces through the ground plane. Altogether there are 41 vias on the board. A high number of vias, but most of them are ground connections.

In my 2-layer board there are seven layers that are important for getting the board manufactured:

  • top copper layer – contains component pads and traces on the top layer
  • top solder mask – contains regions in the top layer that will be exposed for soldering components
  • top silk screen – contains component references and texts on the top layer
  • bottom copper layer – contains component pads and traces on the bottom layer
  • bottom solder mask – contains regions in the bottom layer that will be exposed for soldering components
  • bottom silk screen – contains component references and texts on the bottom layer
  • PCB edges layer – contains the outline of the PCB board

To manufacture the PCB, OSH Park requires Gerber files for all the layers above plus a drill file. The following steps will explain how to create Gerber files in KiCad for OSH Park. I got these information from this blog, but changed a few options to suit my design.

Step 1: Verify DRC (Design Rules Check) with OSH Park specifications.

  • select DRC from the Tools menu or click the ladybug icon in the top bar. Fix any errors in the DRC before proceeding to next step

Step 2: Open the plot dialog box by selecting plot in the File menu or by clicking the printer with a P icon

Step 3: Select the following options in the plot dialog box

Plot dialog box options in KiCad
Plot dialog box options in KiCad

I used the ‘Subtract soldermask from silkscreen’ option to remove the silkscreen from areas where the holes in the solder mask will be. However, even if you didn’t do that OSH Park and most PCB manufacturers will remove the overlapping areas of the silkscreen. But it is better to check for yourself which parts of the silkscreen will be removed.

Step 4: Click the Plot button in the plot dialog box to generate the Gerber files.

Step 5: To open the drill file option box click Generate Drill File from the plot dialog box

Step 6: Select the following drill file options

Generate Drill File dialog box and options in KiCad
Generate Drill File dialog box and options in KiCad

Here, OSH Park requires you to ‘Keep zeros’, use ‘2:4 precision’ and use a ‘Minimal header’.

Step 7: After selecting the correct options in Step 6, click the OK button to generate the drill file which will be in Excellon format.

Step 8: Finally examine each Gerber file and the drill file for errors using the GerbView tool in KiCad.

Here are what my top and bottom side Gerber files look like in GerbView:

Top side copper, solder mask, and silkscreen Gerbers
Top side copper (green), solder mask (blue), silkscreen (white) Gerbers and the drills (purple)
The bottom side copper (green), solder mask (blue) and silkscreen (white) Gerbers

That’s it! I have submitted my board for fabrication to OSH Park, and it cost me $14.35 for three copies. I will add another post when the boards arrive. Meanwhile I have started work on my other spin-off project, which is to create a reflow oven to assemble the surface mount components into the Gyro’clock boards.

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 )

Google+ photo

You are commenting using your Google+ 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 )


Connecting to %s

%d bloggers like this:
search previous next tag category expand menu location phone mail time cart zoom edit close