nand-pcb-test

Homemade PCB test using a CNC router.

Hopefully this is useful to someone else wanting a single place to see the whole CNC PCB building process. These notes assume you have a basic understanding of Kicad and Candle (grblcontrol).

Why?

There are plenty of companies that offer cheap PCB manufacturing, but I'm impatient and bad at designing things correctly on the first try. Imagine ordering a PCB, waiting a few days, and figuring out you messed up your design. Manufacturing with a CNC router helps to eliminate waiting time between idea and implementation.

Alternatively, plenty of people use the chemical etching process (example: thermal transfer paper and ferric chloride) to build their PCBs. I just don't have a good workspace to mess with nasty chemicals, so the CNC approach is more doable for me. Maybe I'll also add a chemical etching bonus section in the future.

For 2+ sided PCBs, it would be worth ordering from a company. Double-sided PCBs are possible, but I have not attempted this yet. I also haven't tried designs with SMD components yet, so that may also be a pain point that warrants ordering PCBs from a company.

Equipment

Build Process

Circuit Design and Prototyping

Design circuit in Kicad Schematic Editor
Breadboard implementation
Protoboard implementation (optional)
Kicad Schematic Editor
- Inspect > Electrical Rules Checker
- Tools > Annotate Schematic
- Tools > Assign Footprints
- File > Plot > PDF, Plot All Pages

PCB Design

Open Kicad PCB Editor (or from Kicad Schematic Editor: Tools > Update PCB From Schematic)
Generally only use back copper and front silkscreen
Rearrange rats nest of components to eliminate overlap
Set design rules (File > Board Setup)
- Minimum clearance: 0.5mm
- Minimum track width: 0.5mm
- Copper to hole clearance: 0.5mm
- Copper to edge clearance: 0.5mm
- Minimum through hole: 0.7mm
- Hole to hole clearance: 0.5mm
Route tracks on B.Cu (back copper) layer. Ignore ground pins, will be filled later
Select Edge.Cuts layer, draw a rectangle to trace board boundary, thickness 1mm
Select B.Cu layer and add fill for ground
Right click fill edge, Zones > Fill Zone
Add orthogonal dimensions to User.Drawings layer to double check board width/height
Place origin at top left of board
Run Design Rules Checker
If exporting F.Silkscreen, I recommend setting text thickness to 0.1mm
Export Gerber files (File > Plot)
- Check Use drill/place file origin
- Export B.Cu, Edge.Cuts (used in router step)
- Export B.Mask (used in solder masking step) as PDF
- Generate Drill Files (*-NPTH.drl and *-PTH.drl)
  - Drill Origin = Drill/place file origin
  - Drill Units = Millimeters
Print (File > Print) F.Silkscreen and F.Mask layers to PDF (used in silkscreen step)
- Verify Print One Page Per Layer is unchecked
- Scale 1:1
- Select Print Mirrored

Bits

Refer to bits listed in Equipment section above.

Isolation routing: 0.5mm pcb milling bit
Holes: 0.8mm drill bit
Edge cut: 2.5mm end mill bit

I know a lot of people seem to recommend v-bits, but I found them to cut too inconsistent to quickly throw together boards.

I did manage to get a couple boards cut with a 0.1mm 60deg bit after manually offsetting my heightmap by 0.05 increments, but I could not replicate this every time. Switching to the pcb milling bit removed ~5-10 minutes of manual adjustment.

Computer Aided Manufacturing (CAM)

Launch FlatCAM
Load B.Cu and Edge.Cuts gerber files (File > Open Gerber)
Add drill files (*.drl) (File > Open Excellon)
- Note: Ignore "No geometry found in file" error if no NPTH holes needed
Options tab
- Set units to mm
Mirror on y-axis since we're cutting the back copper
- Tool > Double-Sided PCB Tool
- Mirror B.Cu and *.drl files on y-axis using Point/Box
Select *-B_Cu.gbr
- Isolation Routing section
- Tool dia: 0.45 (note: 0.05 less than clearance set in Kicad)
- Width (# passes): 2
- Pass overlap: 0.10
- Combine Passes: yes
- Click Generate Geometry
Select *-B_Cu.gbr_iso
- Create CNC Job section
- Cut Z: -0.015
- Travel Z: 2
- Feed Rate: 85.0
- Tool dia: 0.45 (note: 0.05 less than clearance set in Kicad)
- Spindle speed: 10000
- Multi-Depth: yes
- Depth/Pass: 0.08
- Click Generate
Select *-B_Cu.gbr_iso_cnc, export G-Code to B_Cu.nc
Select *-PTH.drl
- If too many sizes of drills, go back to Kicad and change hole sizes of individual components (we can always redrill by hand later if holes too small)
- Create CNC Job section
- Cut Z: -2
- Travel Z: 2
- Feed Rate: 100.0
- Tool Change: no (unless using multiple drill sizes)
- Spindle Speed: 10000
- Click Generate
Select *-PTH.drl_cnc, set tool dia to 0.8, export G-Code to PTH.drl.nc
Select *.Edge_Cuts.gbr
- Board cutout section
- Tool dia: 2.5
- Margin: 0.1
- Gap size: 1.0
- Gaps: 4
- Click Generate Geometry
Select *-Edge_Cuts.gbr_cutout
- Create CNC Job section
- Cut Z: -2
- Travel Z: 2.0
- Feed Rate: 50.0
- Tool dia: 2.5
- Spindle speed: 10000
- Multi-Depth: yes
- Depth/pass: 0.25
- Click Generate
Select *-Edge_Cuts.gbr_cutout_cnc, export G-Code to Edge_Cuts.nc

Preparing Silkscreen

Open F.Silkscreen PDF in Inkscape (to remove blank space of PDF document)
- Select silkscreen components, export
- Export Selection tab, Export Selected Only, 300.0 DPI, SVG

CNC Routing

Refer to bits in "Computer Aided Manufacturing (CAM)" section

To secure the PCB to the bed, I used 3D printed M6 Plate Clamps from https://www.printables.com/model/250450-enhancements-for-sainsmartgenmitsu-3020-pro-max-cn/files. Alternatively, I saw a lot of people using carpet tape.

Probe setup using aluminum tape and z-probe that came with CNC router.

Jog machine to upper left corner, z probe, zero XY
Height map
- Load nc file, click auto
- Zero XYZ, set bit at origin
- Probe grid, set to be ~10mm apart
- Interpolation grid: 20, 20
- zt = 1.0, zb = -1.0
- Click Probe
- Save as height.map
- Click edit mode to leave edit mode
- Verify use heightmap is checked
Remove probes
Load B.Cu.nc
Swap to drill bit, re-zero Z
Load PTH.drl.nc
Swap to edge cut bit, re-zero Z
Load Edge_Cuts.nc

Silkscreen

Load thermal transfer paper into printer
Print F.Silkscreen SVG onto thermal transfer paper (smooth side up)
- Ensure scale is 100%
Tape thermal paper to front of PCB (toner side down)
Use highest setting of dry iron to heat evenly for 2-3 minutes
Apply polycrylic to preserve silkscreen

Final Steps

Use mini drill press to adjust any holes for larger through hole parts
Use 400-600 grit sandpaper and/or steel wool to remove any small burrs on back copper
File down tabs on sides of PCB
Clean off with a bit of isopropyl alcohol
Use multimeter to check all tracks for shorts
Solder components
Clean off any flux with isopropyl

References

About

Homemade PCB test using a CNC router

kicad pcb-manufacturing cnc

MIT License

Languages

Language:KiCad Layout 81.1%Language:KiCad Schematic 18.9%

barrettotte / nand-pcb-test