Microbug Layout

Introduction

The tech club leadership was so impressed with your charger board that they want already want you to start working on another PCB! On the other end of the tech club focus were micro robots, and you've been assigned to complete the layout. Luckily for you, the speccing and schematic creation of the robot have already been completed, the most glorious part of PCB design has been left to you: the layout.

read below!

Check out the HOPE instructor's blog page about the microbug for a better understanding of what it does!

DO read it up before starting the lab!

Lab Instructions


Complete the layout.
Starter project files are avaliable on BCourses.


You are provided with everything but a board layout. Start KiCad, open the project, review the schematic, then move to the Pcbnew layout editor. IMPORT THE BOARD OUTLINE BEFORE PLACEMENT OR ROUTING.
We also highly, highly suggest searching up the datasheets for the parts we choose to understand what they are supposed to do, and faciliate part placement and orientation in relation to the board outline. Not all part placement rules are specificed below. Understanding how things should be oriented is part of the lab. For example, take a look at the battery cell holder on Digikey.

  1. Make sure it falls under BAC's standard capabilities just like in your last design (USB Charger lab).
  2. You are allowed and encouraged to use both sides of the board.
  3. Standard 2 layer board. You are not allowed to design with more than 2 layers.
  4. Do not change schematic, with one exception:
    • You are allowed to swap connections to pins on the microcontroller if it cleans up your routing. Note however, that the board the instructors completed used this exact schematic. If you do swap, please be prepared to explain why, and also point out on the microcontroller datasheet that there is no significant functionality loss in doing so.
  5. You MUST use the provided board outline and component footprints.
    • Exception: you are allowed to change the footprints for the 2 LEDs not being used as the rear caster.
  6. Try to minimize the number of vias used. A suggested maximum is 20.
  7. One of the LEDs must go on in center of the back of the board, facing downwards. It acts as the caster for the robot.
    • All pin headers should be facing up.
    • The other two LEDs should be visible from the top of the PCB.
  8. The two light sensors must be facing downwards on the left and right sides of the caster LED in the back. They are meant to be used as sensors for line following.
  9. Motors must be mounted at the two cutouts on the top side of the board. You should try to align the center of the pads as nicely as you can with the rounded cutouts. The "c" formed by the silkscreen should be on the inside of the board. Take a look at the gif to get a general idea of how the motors are expected to be mounted. Note that the motors the board outline was made for are round.
check out big gif here: https://imgur.com/a/iWrwj3U
  1. Add the IEEE logo (provided as a bitmap image) somewhere on the board with a reasonable size. Instructions below for how to create footprint from bitmap. As with all silkscreen elements, do not have it overlap pads, board edges, or other silkscreen.
    • We also highly suggest adding additional silkscreen to label important connections). One connector is meant to be used with a jumper, can you figure out which one it is?

Checkoff: We're going to be checking for all of the above, in addition to a completed layout with no DRC errors, and BAC DFM report just like last lab.

Important (and late) note: There is one unconnected error that we expect to be in your completed board layout. Hint: look at the datasheet for the battery holder.

How to Import the Board Outline

If you cleverly set your grid size you can get things to line up nicely using the properties panel.

  1. In the Pcbnew layout editor: File -> Import -> Import Graphics. Then select the included microbug_body.dxf. Change the graphic layer to "Edge.Cuts" then click OK.
importing board outline
  1. Click to set down the imported board outline. It should look like so: (placement arbitary, only to show proper imported size)

How to flip parts to the other side of the board

The rear caster LED is required to be facing downwards along with the two light sensors, and we suggest having the battery holder on the bottom as well.

Note: Text SHOULD BE mirrored when on the back.

  1. Hover over the part you want to flip to the other side of the board, then press F (or Right-Click -> Flip).
  2. That's it. Notice how the colors of the footprint silkscreen changes from the color for the top to the color for the bottom.
View -> 3D Viewer for 3D view

How to insert images

Silkscreen art? Copper art? Just, boring logos?

  1. In the main KiCad project window, find the Bitmap to Component Converter (looks like a lowercase 'a' being measured).
  2. Click "Load Bitmap" and select the desired bitmap. For this lab, the "ieee-logo.bmp" should be in folder named "logos".
Imported logo, Bitmap to Component Converter
  1. Note that the imported image is huge (146.6mm by 146.5mm). You can resize by:
    1. Making the image smaller externally, like in Photoshop or something.
    2. Change the Resolution (in Bitmap info, right above the "Load Bitmap" button). Increase the values to have the resulting footprint appear smaller, and reduce to make it bigger. DPI stands for "dots per inch".
  2. Keep format in Pcbnew (you're going to make a footprint object essentially), and select "Front silk screen" in the "Board Layer for Outline" section.
    • If want to do exposed copper art, you should use the "Front solder mask" option. Don't do this for this lab.
  3. Click the "Export" button and save the footprint (.kicad_mod) file into the "microbug-fplib.pretty" folder in the project directory.
  4. Import the footprint directly in Pcbnew, or add a placeholder, no-pin symbol in the schematic and assign as footprint.
adding footprint directly in Pcbnew