Ecosyste.ms: Awesome

An open API service indexing awesome lists of open source software.

Awesome Lists | Featured Topics | Projects

https://github.com/barrettotte/nand-pcb-test

Homemade PCB test using a CNC router
https://github.com/barrettotte/nand-pcb-test

cnc kicad pcb-manufacturing

Last synced: 25 days ago
JSON representation

Homemade PCB test using a CNC router

Awesome Lists containing this project

README 

        
# 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).



assembled front



assembled back



## 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



- [Genmitsu 3020-PRO MAX V2 CNC Router](https://www.sainsmart.com/collections/new-genmitsu-collection/products/3020-pro-max-v2)

  - [3040 Y-Axis Extension Kit](https://www.sainsmart.com/collections/genmitsu-cnc-replacement-upgrade-parts/products/3020-yaxis-extension-kit) (optional)

- [FR-4 Copper Clad PCB Laminate Board, Single Side, 4 x 2.7 inch (10 piece)](https://www.amazon.com/dp/B01MCVLDDZ)

- Bits

  - [0.5mm PCB End Mill Bit](https://www.amazon.com/gp/product/B073RJ3SYZ)

  - [0.8mm PCB Drill Bit](https://www.amazon.com/gp/product/B091FD44Y3)

  - [2.5mm End Mill Bit](https://www.amazon.com/gp/product/B07P84V888)

  - [Assorted PCB Drill Bit Set](https://www.amazon.com/gp/product/B08M5PLF48)

- [Mini Dry Iron](https://www.amazon.com/gp/product/B09YXVWSTQ)

- [Thermal Transfer Paper](https://www.amazon.com/gp/product/B07GLGL2CX)

- [Monochrome Laser Printer](https://www.amazon.com/gp/product/B00NQ1CLTI)

- [Mini Drill Press](https://www.amazon.com/gp/product/B0BKZRD2P7)



cnc router



## 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



breadboard



protoboard



kicad schematic



### 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



kicad pcb



kicad pcb 3d front



kicad pcb 3d back



### 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`



routed pcb



### 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.



cnc probe setup



- 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



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



assembled front



assembled back



## Archive



I tried to do a couple different steps that I hope to try again in the future.

I left my notes in [archive/](archive/).



## References



- [Candle](https://github.com/trasz/grblControl)

- [FlatCAM](http://flatcam.org/)

- [GCODE Reference](https://marlinfw.org/meta/gcode/)

- Youtube

  - [Homemade custom PCB guide using free KiCAD software; Teaching Tech](https://www.youtube.com/watch?v=NgDXPWaA5Ic)

  - [Homemade PCB using thermal transfer paper](https://www.youtube.com/watch?v=aemG_4sDz_Q)

  - [Intro to Kicad; Shawn Hymel](https://www.youtube.com/playlist?list=PL3bNyZYHcRSUhUXUt51W6nKvxx2ORvUQB)

  - [Machining a PCB on the 3-axis CNC Bridgeport Mill; Usagi Electric](https://www.youtube.com/watch?v=AB84_vbH_e8)

  - [Milling PCBs on a Homemade CNC (Part 2): Masking](https://www.youtube.com/watch?v=qIxvXU7KDmE)

  - [Milling Printed Circuit Boards (PCBs) on a Cheap CNC Machine; Matt's Electronics & RC](https://www.youtube.com/watch?v=bQ6_oYZrsjk)

  - [Relay Calculators: Episode 8 - Using FlatCAM and a CNC mill to make PCBs; Usagi Electric](https://www.youtube.com/watch?v=F2FRN5z2S78)

  - [Sainsmart Genmitsu 3020 Pro Max - 300W Spindle & Linear Rails - Build, Test & Review; techydiy](https://www.youtube.com/watch?v=5vaAthrJQm0)