Skip to content

Design process

Electronics design

V0.2 is based on V0.1 with added battery support. The motor driver microstep pins are fixed to HIGH, and the PCB is now double-sided, making it almost half the size in the XY direction.

Fusion Electronics (Eagle) library

How to use libraries:

  1. Download .lbr and upload it into Fusion's Team Hub

  2. Open Library manager > Hub libraries > Sync libraries > Add selected Hub libraries

  3. Place components

    • LDO (3.3V800mA NJM2845DL1-33): Symbol and footprint are equivalent to the one in LDO library
    • 2.1mm DC juck:
      • Fusion library: DC Power Jacks > 694106105102
    • SBR diode (SBR15U30SP5)
      • Footprint: POWERDI5

Custom library

For some parts, no public libraries are available, so a simple library can be created. In this case, those are only used for pad and through-hole placement.

Ref:

Examples:
*In this case they were only used to place pads and holes, without attaching any 3D components.

  1. LM2596 module

    • This library is only used to place 4 through-holes (Planning to use leads (e.g., resistor) for soldering and place insulation spacers)
    • The module can be placed underneath the PCB, saving space and making soldering easier: Swap left and right on the PCB later

    • Pins: +IN, -IN, +OUT, -OUT
    • Modified based on the existing symbol

    • Footprint based on the LM2596 module dimensions
    • Set "Grid Size" each time to ensure accurate dimensions

  2. Mini blade fuse holder

    • This fuse holder is THT and has four through-hole slots.

    • Used the existing fuse symbol

    • PTH Pad was set as 0.8mm Long

  3. TVS diode (SMBJ45CA)

    • Bidirectional (no polarity): symmetrical symbol

    • Based on the dimensions

  4. SBR diode (SBR15U30SP5)

    • Modified based on TVS diode symbol as Schottky diode

    • The bottom left and right pins (anode) are connected

Double-sided PCB design

Hole / Drill / NPTH in Fusion Electronics:

Item Purpose Electrical Connection Plating Notes
Hole (Non-plated through hole, NPTH) Mechanical holes (screws, alignment) No No Purely mechanical hole
Drill Hole size definition — — Diameter setting, not an object
Via Layer-to-layer electrical connection Yes Yes Used for signals or GND
  • While routing, press Spacebar to place a Via that connect top and bottom layers
  • Then, the route automatically switch to the opposite layer and turn the color (red or blue)

PCB via and rivets

  • Via: a small hole that electrically connects copper traces between PCB layers
  • PCB rivets: Hollow copper sleeves used as a simple DIY way to make vias on double-sided boards to provide a top–bottom connection
  • Typical size: 0.6mm and 1.0mm
  • Typical drill sizes: ~0.8–0.9 mm for 0.6 rivets, ~1.5 mm for 1.0mm ones
  • Rivets must still be soldered after flaring to ensure electrical connection

Alternatives:

  • Wire vias (soldered wires through holes)
  • Manufacturer-plated vias

Ref: PCB rivets

Note

The 0.6 mm or 1.0 mm rivets were difficult to find, only the 0.9mm ones were available.

  • 0.9mm copper rivets
  • It seems like drill size should be 1.3 to 1.5 times larger: 1.35 mm holes

Double-sided PCB mill files

I tried using Gerber2Png from FabLab Kerala to generate PNGs for a double-sided PCB following the Documentation.

  • Fusion360: MANUFACTURE > Export Gerber

  • Gerber2Png:

    • Select all .gbr files (after unzipping)
    • Set Double sided and Generate All > Generate PNG
    • Download PNGs

Outcome:

  • It successfully generated "Alignment cut"
  • The PCB successfully fit in 100 x 70 mm copper board with the alignment cut (95.2 x 63.2 mm)
  • Somehow, it doesn't generate PNG for the drill
    • Ref: Kannai's steps (8.4. Export millholes.png)
    • As a workaround, exported the mill holes with board outline as a vector file from Fusion360: Selected DOCUMENT > Print > Print to File (PDF)
    • Opened the PNG and PDF files in Affinity (vector software) and aligned them.
    • Exported the mill holes as a PNG file the same size as the other PNG files.

Other notes

  • Breakout boards such as Pico and A4988 carriers are placed there only for pinout verification purposes and are not required for PCB design.
  • Remove them afterwards to avoid unnecessary DRC violations due to THT pins such as routing between pin sockets.