From Design to Delivery

The full path from a finished layout to boards on your bench, using JLCPCB as a worked example. Other fabs (PCBWay, OSH Park, Aisler…) follow the same flow with different UIs.

Design → DRC → Export files → Upload & review → Choose options → Order → Fabricate → Ship → Customs → You

1. Finalize & run DRC

Before exporting anything, run the tool's Design Rule Check with rules set to your fab's capability sheet (see Common Mistakes & Risks).

• DRC clean against the fab's rules (not just defaults)
• Footprints verified vs datasheets
• Silkscreen, polarity marks, fiducials, test points present
• Board outline (edge cuts) closed and correct

2. Generate the manufacturing outputs

Fabs don't take your native project — they take standard output files. Typically you zip:

File	Format	What it is
Gerbers	RS-274X (.gbr)	Copper, solder mask, silkscreen, paste — one per layer
Drill file	Excellon (.drl)	Hole positions and sizes
BOM	.csv	Bill of materials (only if ordering assembly)
Pick-and-place / CPL	.csv	Part X/Y, rotation, side (only for assembly)

KiCad → JLCPCB

KiCad exports Gerbers + drill from File → Plot / Generate Drill Files, or use the JLCPCB plugin to produce the exact Gerber/BOM/CPL set in one click. Always preview the Gerbers in a viewer before zipping — it's your last cheap check.

3. Upload & review

• Upload the zip; the site renders it in an online Gerber viewer.
• Confirm layer alignment, board size, and that nothing is missing or mirrored.
• The system auto-detects layer count and dimensions — sanity-check them.

4. Choose fabrication options

The common knobs (JLCPCB defaults shown — other fabs are similar):

Option	Typical default	Notes
Base material	FR-4	Standard fiberglass laminate
Layers	2	1–6+ available; more layers cost more
Thickness	1.6 mm	0.6–2.0 mm options
PCB color (solder mask)	Green	Red, blue, black, white, yellow, purple… non-green may add a day
Surface finish	HASL (lead-free)	ENIG (gold, flat) costs more — better for fine-pitch/QFN
Copper weight	1 oz	2 oz for higher current
Via covering	Tented	Cover/plug options
Special	—	Castellated holes, gold fingers, impedance control (extra)

Color & finish are not just cosmetic

ENIG gives a flat, solderable gold surface — choose it for fine-pitch parts; HASL is cheaper but slightly uneven. Dark solder masks (black) can make rework/inspection harder.

5. Assembly (PCBA) — optional

PCB vs. PCBA

• PCB = the bare board — copper, mask, silkscreen, holes. No parts on it.
• PCBA = PCB + Assembly — the board with components soldered on, ready to use.

You can order just the PCB and hand-solder, or order a full PCBA and get a populated board.

If you don't want to hand-solder, fabs offer SMT assembly:

• Provide the BOM + pick-and-place (CPL) files.
• Parts come from the fab's library (JLCPCB uses LCSC). Basic parts are cheapest; Extended parts add a per-reel loading fee.
• You usually assemble one side (SMT); through-hole or both sides may cost more.

PCBA risks to check before ordering

Assembly adds failure modes a bare PCB doesn't have — most are cheap to catch now, expensive after a run:

• Wrong footprint → part won't fit or won't solder. Fix: verify pad size/pitch vs the datasheet, not just a library symbol.
• Wrong orientation / rotation → the assembler places pin 1 the wrong way → dead or destroyed parts. Fix: check polarity marks (diodes, electrolytics, ICs) and confirm the rotation in the CPL file — the part's rotation in your library often differs from the fab's expectation (a classic JLCPCB gotcha; preview placement before confirming).
• Low stock / out-of-stock parts → the chosen part runs out before/at assembly → order delayed or partially populated. Fix: check live stock when picking parts; prefer Basic/in-stock parts; have an alternate part number ready.
• End-of-life (EOL) / long lead-time parts → fine for one prototype, risky for any repeat build. Fix: avoid EOL parts; note lead times for anything critical.
• MOQ & extended-part fees → small quantities can carry minimum-order and per-reel loading costs. Fix: factor these into the quote.

Lock your BOM to real, in-stock parts

A board designed around a part that's out of stock (or EOL) can stall the whole order. Pick parts that show healthy live stock, prefer the fab's basic/preferred library, and keep a backup part number for anything important.

6. Place the order

• Set quantity (5 pcs is the common minimum for prototypes) and build time.
• Review the auto-quote (board + assembly + shipping).
• Pay; fabrication for a standard 2-layer board is often ~24–48 h.

Approximate prototype cost

A standard 2-layer board (≤100×100 mm, green, 1.6 mm, HASL) is frequently a few US dollars for 5 pieces — shipping usually costs more than the boards. Prices and promos change; check the live quote.

7. Shipping

• Choose a courier (e.g. DHL/FedEx-type express, or cheaper economy/post).
• Express is days; economy can be weeks. You get a tracking number.
• Total time ≈ fabrication + shipping — plan around both.

8. Import / export & customs

General guidance only — verify for your country

The following is a rough, non-authoritative overview. Rules vary by country and change; confirm with the carrier or local customs/import authority, and with your institution if ordering through it.

• Customs duties / import VAT/GST may apply depending on your country and the declared value; some places exempt low-value parcels, others don't.
• The courier often handles clearance and may collect duties/fees on delivery — budget for this.
• Customs inspection can add delays; keep the commercial invoice and order details handy.
• Declared value, contents and HS codes are set on the shipping documents; under-declaring value is potentially a violation — avoid it.
• For ordinary hobby/research boards this is usually routine, but sensitive or controlled designs (certain RF, cryptographic, or defense-related hardware) could potentially fall under export-control regulations — check before sending designs abroad.
• If ordering for the lab/university, there may be institutional procurement or import rules — ask first.

JLCPCB case study (typical prototype)

1. Finish layout in KiCad, run DRC against JLCPCB capabilities.
2. Export Gerbers + drill (or one-click via the JLCPCB plugin); zip them.
3. Upload to JLCPCB → check the Gerber viewer.
4. Options: 2-layer, FR-4, 1.6 mm, green, HASL lead-free, 1 oz, 5 pcs.
5. (Optional) Add SMT assembly with BOM + CPL from LCSC parts.
6. Order → fabrication ~24–48 h → ship by chosen courier → arrives after customs.

Cost optimization

Most of the price is decided by a handful of choices. Pick the cheapest option that still meets your reliability needs.

What drives PCB price

Driver	Effect on price	Cheaper choice
Layer count	Biggest single jump (2 → 4 → 6)	Stay at 2 layers if it routes
Board area	Bigger board = more	Shrink layout; stay within size brackets (e.g. ≤100×100 mm)
Min trace/space & via/hole	Tight rules push you into a pricier "advanced" tier	Keep standard (≥ 6 mil track, ≥ 0.3 mm via)
Surface finish	ENIG > HASL	HASL unless you need fine-pitch/QFN
Solder mask color	Non-green may add time/cost	Green
Copper weight	2 oz > 1 oz	1 oz unless high current
Thickness	Non-standard costs more	1.6 mm
Special features	Via-in-pad, blind/buried vias, impedance control, castellated, gold fingers each add cost	Avoid unless required
Build time	Faster = more	Standard lead time
Quantity	Price breaks per board	Batch with labmates

Via size is a price tier, not just a rule

Asking for very small vias/holes or thin traces moves the whole board into the fab's advanced process — more expensive and lower yield. Use standard via sizes unless the part pitch genuinely forces smaller. See Common Mistakes & Risks.

What drives PCBA (assembly) price

• One side vs two sides of SMT → single-sided is cheaper → put all SMT parts on one side.
• SMT vs through-hole → THT usually means extra hand-soldering cost → prefer SMT parts.
• Unique part count & total placements → fewer unique parts = less setup.
• Basic vs Extended parts (JLCPCB) → Extended parts add a per-type loading fee; Basic parts don't → prefer Basic/preferred parts.
• Stencil & setup fees → fixed costs that amortize over larger quantities.

Quick wins

• Stay at 2 layers + standard design rules whenever routing allows.
• Keep all SMT components on one side of the board.
• Prefer Basic / in-stock parts; minimize unique part numbers.
• Green mask + HASL + 1.6 mm + 1 oz is the cheapest standard stack.
• Not urgent? Pick economy shipping and standard build time.
• Batch orders with labmates to clear minimums and split shipping.

Don't optimize past reliability

Cheaper isn't always better. Choose ENIG for fine-pitch/QFN, 2 oz copper for power, or 4 layers when signal integrity needs a solid reference plane. A few extra dollars here prevents a respin — which is the real cost.

References

• KiCad documentation — plotting Gerbers and drill files.
• Fab capability & ordering guides — e.g. JLCPCB, PCBWay, OSH Park.
• See also: PCB Design Software (EDA Tools) · Common Mistakes & Risks.