My First KiCad Board!

Posted by: Dave Vandenbout 6 years, 3 months ago

(1 comment)

I made the decision last year to move from Eagle to KiCad. I got tired of releasing OSHW boards that many people couldn't modify because the freeware version of Eagle was so limited. I also got tired of paying $600 for upgrading to the next major release, especially when the big, new feature was ASCII-encoded design files. Really, that's it?! Hold me back!

I got a taste of the KiCad design flow by watching Chris Gammel's "Getting to Blinky" video series while I was sitting in a hospital waiting room. Chris's videos made the time pass so quic ... nope, still bored. Though it was a better use of the time than folding and reorganizing the disposable hospital gowns. Damn you, OCD!

But eventually, as I learned in grad school, you have to stop reading stuff and start doing stuff. So last week, I downloaded and installed the latest development version of KiCad for Windows. (My philosophy is, if you're going to learn to drive, it might as well be on a car where the brakes don't work.) It takes a while to build KiCad, but having the source available can be important (as I'll discuss later).

As my first project, I decided to build a StickIt! module for an eight-channel ADC chip, the TI ADC108S. StickIt! modules are small (2.0" x 8") and usually only need a two-layer PCB, so I figured this would be easier than a four-layer PCB with a 256-ball BGA.

I used KiCad's Eeschema tool to enter the schematic shown below. It works pretty much like most schematic editors I've used. (However, I was never able to figure out how to globally rename a net; I had to click on each stub where the net name was used and rename it.) I also learned how to define new parts for the schematic because, as usual, the parts you need are never in the libraries. (I also checked at the KiCad CLoud parts repository. No luck.)

Going from a schematic to laying out the PCB isn't as seamless in KiCad as it is in Eagle. You have to:

1. Generate the netlist from the schematic.
2. Associate footprints with each schematic symbol using the CvPCB tool.
3. Regenerate the netlist from the schematic (to incorporate the footprint assignments).
4. Start PCBnew and import the netlist.

There's also no live-link between the schematic and the PCB layout, so you can't highlight a net in the schematic and then see it in the layout. Still, it gets the job done.

The steps for using PCBnew aren't much different from any other layout tool:

1. Specify your board parameters: # of layers, minimum trace/space, solder mask clearance, etc. (PCBnew has these parameters spread around between the Dimensions and Design Rules menus, so it's kind of confusing.)
2. Define the board boundary using what KiCad calls the Edge Cuts layer. (Really, can't we all use the same terminology? PCB design is like 100 years old.)
3. Place the parts. (PCBnew has a nice feature where all the air wires are hidden except those connected to the part you're currently moving.) There's an auto-placement feature as well, but I didn't find out about that until I finished the layout.
4. Place copper-pour polygons for ground and power planes. (You can also put cutouts into the planes, which is something I couldn't do in Eagle.)
5. Draw the wiring traces. (Real-time design-rule checking prevents you from getting traces too close, but this feature can be turned off when you want to ram a trace through and clean up the design violations later.) There's also a button for doing autorouting using the FreeRouting web service.
6. Run a design rule check. (The DRC also calculates the fill-in for the copper-pours, which seems weird to me. It took me a while to find out that was how to redraw the pours.)

Here's the front and back layouts for my first board:

One of the pain points for the layout was, oddly enough, generating the graphics for the back-side of the PCB. KiCad provides the Bitmap2Component tool for translating any of around twenty different graphic file formats into a footprint you can place in a silkscreen layer. It produces a much smaller, easier-to-handle file than the equivalent tool in Eagle. But it's limited in that there's no way to scale the footprint: it uses a fixed resolution of 300 dpi, so if your image is 1200 pixels wide, it will be 4 inches wide on the board. I had to write a small Python script to scale all the polygon vertices in the .kicad_mod file that was generated by the tool. (It's nice that all the KiCad files are ASCII text and have well-structured formats that are easy to parse.)

I had a problem getting PCBnew to find the new footprint; it kept reporting "library module path does not exist." Since the error message was providing a .c file and a line number where the problem was found, I could check the source to see if I could find a solution. From that I was able to determine that I only needed to provide the directory for footprint files of type .kicad_mod and not the file itself.

Another problem was that when I placed the graphics footprint on the backside of the PCB, I was unable to mirror it. That meant the text would read backwards when the board was flipped over. I solved the problem by using a negative scaling factor for the X coordinate in my Python script. It was only while writing this post that I found I had to do the mirroring of the footprint in the Module Editor instead of PCBnew, but even then it doesn't seem to be working for me.

Once the layout was done, I generated the Gerber files for the PCB fabricator. (This function is under the File => Plot menu instead of the File => Fabrication Outputs menu where you can, however, generate the drill file. WTF?) I checked the Gerber files with the GerbView tool and also using the free version of ViewMate from PentaLogix. The results seem to match, but the Y coordinate-mapping translates the layout below the X-axis. I can't find a way to change that. I guess I'll see if that has any effect when the boards are made. At least the drills and the wire traces match up.

Now that the boards are sent for fabrication, how would I rate the whole experience? Good, overall. KiCad has its quirks, just like Eagle. (I think the designers of both must have attended Crazy Eddie's UX Design School.) In most cases, I think my problems were caused by inexperience and will lessen once KiCad gets into my muscle memory.

If I were starting to do PCB design from scratch today and needed to select a design tool, I would pick KiCad over Eagle. Here's why:

• KiCad tools are equivalent and of about the same quality (sometimes better) as those found in Eagle.
• KiCad is free. Eagle Professional (which is the only version that doesn't limit your board size and the number of layers) is $1640 (you do get their autorouter with that, but I've never heard of anybody who likes it).
• KiCad is open source. That won't matter to a lot of people, but it helps sometimes when you're looking for the source of a problem and you'd like it fixed sometime during this century.
• KiCad is starting to support Python scripting. This will be incredibly powerful and much nicer than working with the User Language Programming tool found in Eagle. It should make re-creating my BOM pricing tool much easier.
• Along with the open source community, CERN has started putting some design effort into KiCad. This increases the momentum of KiCad development and serves as some validation for its usefulness.

Besides, how can you not like a tool that gives you 3D board visualizations right out of the box!

• ← Thanks Bunches for That!
• Test Results for My First KiCad Board! →