Now that you have your USB charger designed and parts picked out, you can start the layout right? Not so fast! There are a couple more things to consider.
Reviewing component footprints
Do you have a footprint for everything? If you haven’t already done so, from the schematic you’ll need to map every symbol to a physical footprint that matches the physical part you chose. Usually most footprints you run across will be standardized ones that are in the KiCAD library already. However, in the off chance you have some somewhat special part that doesn’t already exist, you’ll need to make your own just like how custom symbols are made. We've made a tutorial on how to do this here.
While we didn't really think of this during the component selection process, it's important to keep in mind the size of all the parts and the final PCB. Does everything fit on the board, where you want them to go?
Optional: A fun exercise in making custom footprints would be to make this switch. It's relatively complicated dimensionally, and if you can make this you can probably make any footprint. Land pattern on the right, from the datasheet.
Design Rule review
Is everything okay for standard manufacturing? The board manufacturer that sponsors this class is Bay Area Circuits, and as a result, we need to follow their manufacturing capabilities for our boards to be made. In KiCAD we can set up the rules that our design must follow under File > Board Setup. Then click on Design Rules, and then fill in the values according to this table of capabilities. There is also a subcategory under Design Rules called Net Classes, and you can set different rules for different types of nets (e.g. power should have a thicker minimum width).
For your convenience, under Tracks & Vias, you should fill out some standard track widths and via sizes so during actual routing you can quickly switch between your values. Some “normal” widths would be like 6 mils, 8 mils, 10 mils, 12 mils, 15 mils, 20 mils, and 25 mils. Similarly for vias, set up some nice round numbers from the minimum via size upwards (making sure the size is 2x the drill).
We would like for you charging components to fit within a specific board outline so that it fits perfectly on top of a battery holder. Below the picture of the battery holder are two different outlines you can make, the second of which is much smaller and potentially harder to get everything to fit.
Normal Version (with one passthrough hole)
You will need to use a Horizontal USB receptacle. The total height should not exceed 10mm (board + components).
You will need to use a VERTICAL USB receptacle for this version.
No components should extend beyond the USB receptacle.
What's in a layout?
Now you have all your parts and their footprints imported into an outline you've drawn, it's time to begin putting all the parts in reasonable places and begin routing.
- USB port needs to be accessible: should probably be on the edge if it is a horizontal receptacle
- Group together parts like in your block diagram before routing
- Route ground with a plane
- Don't forget you have two sides to route on
Optional: You can output the board as a 3D model file (a .step). Does it match up to a 3D modeled enclosure?
For the actual checkoff:
- Have correct design rule set up
- Have a fully routed layout that fits in one of the above outlines
- Not just 0 unrouted, but everything is routed well (using planes, no wild loops, etc).
- In the 3D view the height of the design is within specified limits
- Run DRC and show your design passes
Optional: If you wanted to get this board actually made, you will need to export something called Gerbers. This is a set of files that the actual manufacturer can read for fabrication. Under File > Plot, you'll get a window to output Gerbers. The exact format to use will depend on manufacturer, but you need to export all the relevant layers and drill files. Bay Area Circuits has a handy online serivce to check your Gerbers are within their design capabilities here.