Week 8 — Group Assignment: Electronics Production

Group assignment brief

Characterise how we make PCBs at Chaihuo — both in-house and through a board house:

• Characterize the design rules for our in-house PCB production process and document the machine settings
• Document the workflow for sending a PCB design to a board house
• Document the work on this group page; each student reflects on what they learned when completing the individual assignment (make and test an embedded system you designed)

See assignment requirements for the full brief.

This page documents our Week 8 group collaboration at Chaihuo Makerspace: milling PCBs on the lab KEXU CNC, finding working parameters, and ordering the same design from JLCPCB. PCB layouts came from the Week 6 electronics-design work.

In-House PCB Milling

Machine — KEXU (Exu Turbo)

Our in-house PCB production uses the KEXU desktop CNC at the Small CNC & Drill Press area. Instructor Matthew walked the group through safety and setup before the first cut.

Specification	Details
Model	Exu Turbo (3-axis)
Overall dimensions (L × W × H)	550 × 490 × 620 mm
Travel (X / Y / Z)	190 × 120 × 110 mm
Relief carving area	200 × 120 mm
Spindle speed	0 – 24,000 rpm
Spindle power	800 W, water-cooled
Machining speed	0 – 4000 mm/min
Tool holder capacity	1 – 6 mm
Control	7-inch touch screen (Wi-Fi / USB)

Safety: wear a mask and safety goggles when milling FR-4 — the dust is fine and should not be inhaled.

Material and tools

Item	Specification
Substrate	FR-4 epoxy glass fibre (single-sided copper)
Board thickness	1.5 – 1.6 mm
Copper thickness	35 μm (1 oz)
Trace bit	40° #502 V-bit
Outline bit	4-flute end mill (~1.5 mm)

Design rules and machine settings

We tested different feed/speed/depth combinations until traces were clean and outlines cut through without snapping the bit. These are the parameters we settled on:

Parameter	V-bit (tracing)	Ball-end / end mill (outline)
Feed speed	4 mm/s	4 mm/s
Spindle speed	14,000 rpm	14,000 rpm
Offset number	4	4
Offset stepover	0.2 mm	0.2 mm
Cut depth	0.23 mm	0.45 mm
Tool diameter (effective)	0.3 mm	1.5 mm

The 0.23 mm trace depth removes copper without cutting too deep into the substrate. The 0.45 mm outline depth per pass cuts through the board in several passes without overloading the bit.

Practical design limits for in-house milling:

Rule	Value / note
Minimum reliable trace/space	~0.38 mm
Trace width recommendation	1 mm for power buses; 0.5 mm signal traces can be fragile after milling
Isolation routing	Multiple offset passes (4 × 0.2 mm stepover)
Board fixturing	Double-sided tape on sacrificial layer; board must stay flat
Z zero	Lower bit until it just touches copper (paper / tape drag test), then set Z = 0
File transfer	FAT32 USB; avoid hyphens in filenames — the controller rejects them

Milling workflow

The full in-house workflow at Chaihuo:

1. Design in KiCad (schematic + PCB from Week 6)
2. Export Gerber — at minimum F_Cu.gbr (traces) and Edge_Cuts.gbr (outline) for milling
3. Convert to PNG — use gerber2png or KiCad plot
4. Generate G-code in Mods — upload PNG on the Mods CE, select 40° V-bit for traces and end mill for outline, simulate, save .nc
5. Load on machine — copy .nc files to USB, select trace file first then outline
6. Zero and run — set X/Y at board corner, Z on copper surface; start with conservative depth and adjust if the first pass looks shallow
7. Deburr and clean — scrape loose copper with a steel ruler; wash with soap and water to remove oils

Mods browser compatibility

Use Chrome or Edge with Mods. Some browsers (e.g. Brave) produce bad toolpaths — unwanted dots or irregular patterns.

Machine setup (photos)

Install the V-bit in the collet and tighten with the wrenches provided.

Secure the copper-clad board on the sacrificial layer with tape or a toe clamp. Jog the spindle to the front-left corner for X/Y zero.

Set X, Y, Z zero on the touch-screen controller:

Axis	Method
X, Y	Move tool to front-left corner of copper board → Set XY Zero
Z	Lower until bit touches copper (paper drag test) → Set Z Zero

Select the G-code file from USB (TRACE.NC, outline file) and run. Pause and re-zero Z if the first pass is too shallow or too deep.

Laser cutting (explored, not recommended)

We also tested LaserPecker 3 (diode laser) for copper removal. With negative SVG plots from KiCad (white = keep traces, black = remove copper), a single pass took ~10 minutes but did not fully isolate the traces even after multiple passes. A fibre laser can remove copper in fewer passes; our diode laser is useful for marking but not reliable as a primary PCB fabrication method. Vinyl cutting was explored separately by other students — see Emily's documentation linked from Timothy's Week 8 page.

Submitting a PCB to a Board House

In-house milling is fast for prototyping (roughly one hour per board) but limited to ~0.38 mm features and produces boards without solder mask or silkscreen. When we need cleaner boards, tighter spacing (~0.125 mm), or more than a handful of copies, we send the design to a board house.

Files needed

Milling only needs two Gerber layers. A board house needs the full fabrication package:

File	Purpose
F_Cu.gbr	Front copper traces
Edge_Cuts.gbr	Board outline
F_Mask.gbr	Front solder mask (exposes pads only)
B_Mask.gbr	Back solder mask (often includes drill info)
F_Silkscreen.gbr	Component labels and polarity marks
.drl (or embedded in mask)	Drill locations, sizes, plated vs non-plated

Solder mask is the coloured polymer coating that protects copper and prevents solder bridges. Silkscreen prints reference designators (R1, C2, …) on the surface for assembly. Both are generated from the same KiCad design used in Week 6 — export via File → Fabrication Outputs → Gerbers.

Ordering at JLCPCB

Instructor Matthew introduced JLCPCB (JLC Technology Group, Shenzhen) as a fast, low-cost option for our cohort. Workflow:

1. Export and zip all Gerber + drill files from KiCad
2. Upload the zip to jlcpcb.com
3. Review auto-detected parameters — board size, layer count, thickness; adjust if needed
4. Confirm the preview — side-by-side design vs production draft plus 3D view; last chance to catch layer errors
5. Pay and wait — production typically starts within a day; delivery to Shenzhen is 2–7 days depending on courier

Typical order settings for our development boards:

Parameter	Value
Board material	FR-4
Layer count	2
Board thickness	1.0 – 1.6 mm
Surface finish	Lead-free HASL
Electrical test	Flying probe (free)
Quantity	5 boards

Our group orders came to roughly ¥40 RMB (~$6 USD) for 5 boards plus shipping. One order placed 23 March arrived 25 March; another cohort order (via JLCPCB from Timothy's test) cost $5.56 for 5 boards with shipping to Shenzhen — delivery took 7 days because the courier required an answered phone call before drop-off.

Milled vs board-house boards

	In-house (KEXU)	Board house (JLCPCB)
Turnaround	~1 hour	2–7 days
Trace quality	Good for ≥0.38 mm; edges rougher	Clean, consistent
Solder mask	None	Green (or other colour)
Silkscreen	None	Reference designators printed
Best for	Rapid iteration, debugging	Cleaner assembly, final-ish prototypes

Both methods have a place: mill first to validate the design, then order from JLC when the layout is stable.

What We Learned

• Measure and zero carefully. A board that is not flat or a Z zero that is slightly off produces shallow traces or cuts into the sacrificial layer.
• In-house rules are tighter than board-house rules. Design for ≥0.38 mm traces/spacing when milling; use wider buses where possible.
• Mods + a post-processor bridge the gap between MIT's toolchain and our KEXU controller — always simulate in Mods and test-cut before committing copper.
• Board-house export is a different mindset. Solder mask, silkscreen, and drill files each serve a fabrication step you do not think about when milling.
• Check the JLC preview. The 3D render catches mirrored layers and missing drill files before they become expensive mistakes.
• Clean the milled board before soldering — remove tape residue and wash off FR-4 dust.

These group findings feed directly into each student's individual assignment: populate and test the embedded system on either a milled or ordered board.