Part 8: Manufacturing Files

Manufacturing Workflow

Your PCB design is only data until a fabricator turns it into copper and fiberglass. The quality of your manufacturing output files directly determines whether you get back exactly what you designed — or a board full of errors.

flowchart LR
    A["PCB Design
(EDA tool)"] --> B["Generate Gerbers
+ Drill Files"]
    B --> C["Generate BOM
+ PnP Data"]
    C --> D["Review &
Verify Files"]
    D --> E["Upload to
Fabricator"]
    E --> F["Bare PCB
Fabrication"]
    F --> G["SMT Assembly
(if ordered)"]
    G --> H["Boards
Delivered"]
                            

Manufacturing File Formats

Gerber Files

Layer Mapping

Gerber RS-274X is the industry standard for PCB fabrication data. Each physical layer of your PCB gets its own Gerber file. Here is the standard layer mapping for a 4-layer board:

KiCad Gerber Export

# KiCad CLI Gerber export (KiCad 8+)
# Generate all manufacturing files from the command line

# 1. Generate Gerbers
kicad-cli pcb export gerbers \
    --output ./gerbers/ \
    --layers "F.Cu,In1.Cu,In2.Cu,B.Cu,F.Mask,B.Mask,F.SilkS,B.SilkS,F.Paste,B.Paste,Edge.Cuts" \
    --subtract-soldermask \
    --use-drill-file-origin \
    my_project.kicad_pcb

# 2. Generate drill files (Excellon)
kicad-cli pcb export drill \
    --output ./gerbers/ \
    --format excellon \
    --drill-origin plot \
    --excellon-units mm \
    --generate-map \
    my_project.kicad_pcb

# 3. Generate pick-and-place CSV
kicad-cli pcb export pos \
    --output ./assembly/placement.csv \
    --format csv \
    --units mm \
    --side both \
    my_project.kicad_pcb

# 4. Generate BOM
kicad-cli sch export bom \
    --output ./assembly/bom.csv \
    my_project.kicad_sch

echo "Manufacturing files generated in ./gerbers/ and ./assembly/"

Gerber Verification

# Gerber file package verifier
# Checks that all required files exist before upload

import os

required_files = {
    "Top Copper":       ["F_Cu.gbr", ".gtl"],
    "Bottom Copper":    ["B_Cu.gbr", ".gbl"],
    "Top Solder Mask":  ["F_Mask.gbr", ".gts"],
    "Bottom Solder Mask": ["B_Mask.gbr", ".gbs"],
    "Top Silkscreen":   ["F_SilkS.gbr", ".gto"],
    "Board Outline":    ["Edge_Cuts.gbr", ".gko", ".gm1"],
    "Drill File":       [".drl", ".xln"],
}

gerber_dir = "./gerbers"  # Change to your output directory

print("Gerber Package Verification")
print("=" * 50)

all_files = os.listdir(gerber_dir) if os.path.isdir(gerber_dir) else []
missing = []

for layer, patterns in required_files.items():
    found = any(
        any(f.endswith(ext) or ext.lstrip('.') in f for f in all_files)
        for ext in patterns
    )
    status = "✓ Found" if found else "✗ MISSING"
    if not found:
        missing.append(layer)
    print(f"  {layer:>22}: {status}")

print(f"\nTotal files in directory: {len(all_files)}")
if missing:
    print(f"⚠ MISSING LAYERS: {', '.join(missing)}")
    print("DO NOT upload until all layers are present!")
else:
    print("✓ All required layers present — ready to upload")

Gerber Package Verification
==================================================
            Top Copper: ✓ Found
         Bottom Copper: ✓ Found
       Top Solder Mask: ✓ Found
    Bottom Solder Mask: ✓ Found
       Top Silkscreen: ✓ Found
        Board Outline: ✓ Found
           Drill File: ✓ Found

Total files in directory: 11
✓ All required layers present — ready to upload

Drill & Route Files

Excellon Drill Format

Excellon is the standard drill data format. It specifies tool definitions (drill sizes) and hole coordinates. Modern tools use Excellon format 2.4 (2 integer digits, 4 decimal digits, millimeters).

# Example Excellon drill file structure
# M48 = header start
# T1C0.300 = Tool 1, 0.300mm diameter
# % = end of header
# T1 = select tool 1
# X25400Y50800 = drill at (25.4mm, 50.8mm)

# Common drill sizes for embedded PCBs:
# 0.3mm  - Standard vias
# 0.4mm  - Power vias
# 0.8mm  - Through-hole header pins (0.1" pitch)
# 1.0mm  - Mounting holes (M2)
# 1.1mm  - Through-hole components
# 3.2mm  - Mounting holes (M3)

Drill Verification

# Drill file analyzer — count holes by size
drill_tools = {
    "T1": {"size_mm": 0.30, "count": 245, "type": "Via"},
    "T2": {"size_mm": 0.40, "count": 48,  "type": "Power Via"},
    "T3": {"size_mm": 0.80, "count": 80,  "type": "Header Pin"},
    "T4": {"size_mm": 1.00, "count": 4,   "type": "M2 Mount"},
    "T5": {"size_mm": 1.10, "count": 12,  "type": "Through-Hole"},
    "T6": {"size_mm": 3.20, "count": 4,   "type": "M3 Mount"},
}

print("Drill File Analysis")
print("=" * 60)
print(f"{'Tool':>6} | {'Size (mm)':>9} | {'Count':>6} | {'Type':>15}")
print("-" * 60)

total_holes = 0
for tool, info in drill_tools.items():
    total_holes += info["count"]
    print(f"{tool:>6} | {info['size_mm']:>7.2f}mm | {info['count']:>6} | {info['type']:>15}")

print(f"\nTotal drill hits: {total_holes}")
print(f"Unique tool sizes: {len(drill_tools)}")
print(f"\nTip: Fewer unique drill sizes = faster fabrication")
print(f"Tip: Minimum via size for standard fab: 0.3mm (12 mil)")

Drill File Analysis
============================================================
  Tool | Size (mm) |  Count |            Type
------------------------------------------------------------
    T1 |   0.30mm  |    245 |             Via
    T2 |   0.40mm  |     48 |       Power Via
    T3 |   0.80mm  |     80 |      Header Pin
    T4 |   1.00mm  |      4 |        M2 Mount
    T5 |   1.10mm  |     12 |    Through-Hole
    T6 |   3.20mm  |      4 |        M3 Mount

Total drill hits: 393
Unique tool sizes: 6

Tip: Fewer unique drill sizes = faster fabrication
Tip: Minimum via size for standard fab: 0.3mm (12 mil)

Bill of Materials (BOM)

Production BOM Format

A production BOM includes everything the assembler needs: component value, package, manufacturer part number (MPN), supplier, and quantity.

BOM Cost Estimator

# BOM cost estimator for prototype and production quantities
bom = [
    {"ref": "U1",      "value": "STM32F411CEU6", "pkg": "UFQFPN-48", "qty": 1, "unit_1": 3.50, "unit_1k": 2.80},
    {"ref": "U2",      "value": "AMS1117-3.3",   "pkg": "SOT-223",   "qty": 1, "unit_1": 0.15, "unit_1k": 0.08},
    {"ref": "Y1",      "value": "8MHz Crystal",   "pkg": "3215",      "qty": 1, "unit_1": 0.30, "unit_1k": 0.15},
    {"ref": "R1-R10",  "value": "10kΩ 0402",      "pkg": "0402",      "qty": 10,"unit_1": 0.01, "unit_1k": 0.003},
    {"ref": "C1-C15",  "value": "100nF 0402",     "pkg": "0402",      "qty": 15,"unit_1": 0.02, "unit_1k": 0.005},
    {"ref": "C16-C18", "value": "10µF 0805",      "pkg": "0805",      "qty": 3, "unit_1": 0.05, "unit_1k": 0.02},
    {"ref": "L1",      "value": "Ferrite 0805",   "pkg": "0805",      "qty": 1, "unit_1": 0.08, "unit_1k": 0.03},
    {"ref": "J1",      "value": "USB-C Connector", "pkg": "USB-C",    "qty": 1, "unit_1": 0.50, "unit_1k": 0.30},
    {"ref": "J2",      "value": "SWD 1.27mm 2x5", "pkg": "2x5 1.27", "qty": 1, "unit_1": 0.40, "unit_1k": 0.20},
]

print("BOM Cost Analysis")
print("=" * 80)
print(f"{'Reference':>10} | {'Value':>18} | {'Qty':>4} | {'Proto @1':>9} | {'Prod @1k':>9}")
print("-" * 80)

total_proto = 0
total_prod = 0
total_parts = 0

for item in bom:
    proto_cost = item["qty"] * item["unit_1"]
    prod_cost = item["qty"] * item["unit_1k"]
    total_proto += proto_cost
    total_prod += prod_cost
    total_parts += item["qty"]
    print(f"{item['ref']:>10} | {item['value']:>18} | {item['qty']:>4} | ${proto_cost:>7.2f} | ${prod_cost:>7.2f}")

print("-" * 80)
print(f"{'TOTAL':>10} | {'':>18} | {total_parts:>4} | ${total_proto:>7.2f} | ${total_prod:>7.2f}")
print(f"\nPCB fabrication (5 pcs, JLCPCB):    ~$5.00")
print(f"Assembly (5 pcs, JLCPCB):            ~$15.00")
print(f"Total prototype cost (5 boards):     ~${5*total_proto + 5.00 + 15.00:.2f}")

BOM Cost Analysis
================================================================================
 Reference |              Value |  Qty |  Proto @1 |  Prod @1k
--------------------------------------------------------------------------------
        U1 |     STM32F411CEU6 |    1 |    $3.50  |    $2.80
        U2 |      AMS1117-3.3  |    1 |    $0.15  |    $0.08
        Y1 |    8MHz Crystal   |    1 |    $0.30  |    $0.15
    R1-R10 |     10kΩ 0402     |   10 |    $0.10  |    $0.03
    C1-C15 |    100nF 0402     |   15 |    $0.30  |    $0.08
   C16-C18 |     10µF 0805     |    3 |    $0.15  |    $0.06
        L1 |   Ferrite 0805    |    1 |    $0.08  |    $0.03
        J1 | USB-C Connector   |    1 |    $0.50  |    $0.30
        J2 |  SWD 1.27mm 2x5  |    1 |    $0.40  |    $0.20
--------------------------------------------------------------------------------
     TOTAL |                   |   34 |    $5.48  |    $3.73
PCB fabrication (5 pcs, JLCPCB):    ~$5.00
Assembly (5 pcs, JLCPCB):            ~$15.00
Total prototype cost (5 boards):     ~$47.40

BOM Cost Analysis
================================================================================
 Reference |              Value |  Qty |  Proto @1 |  Prod @1k
--------------------------------------------------------------------------------
        U1 |     STM32F411CEU6 |    1 |    $3.50  |    $2.80
        U2 |      AMS1117-3.3  |    1 |    $0.15  |    $0.08
        Y1 |    8MHz Crystal   |    1 |    $0.30  |    $0.15
    R1-R10 |     10kΩ 0402     |   10 |    $0.10  |    $0.03
    C1-C15 |    100nF 0402     |   15 |    $0.30  |    $0.08
   C16-C18 |     10µF 0805     |    3 |    $0.15  |    $0.06
        L1 |   Ferrite 0805    |    1 |    $0.08  |    $0.03
        J1 | USB-C Connector   |    1 |    $0.50  |    $0.30
        J2 |  SWD 1.27mm 2x5  |    1 |    $0.40  |    $0.20
--------------------------------------------------------------------------------
     TOTAL |                   |   34 |    $5.48  |    $3.73
PCB fabrication (5 pcs, JLCPCB):    ~$5.00
Assembly (5 pcs, JLCPCB):            ~$15.00
Total prototype cost (5 boards):     ~$47.40

Pick-and-Place Data

Pick-and-place (PnP/CPL) files tell the SMT machine exactly where to place each component. The file contains the reference designator, X/Y coordinates, rotation angle, and board side.

# Pick-and-place file format (JLCPCB compatible)
# Columns: Designator, Val, Package, Mid X, Mid Y, Rotation, Layer

pnp_data = [
    ("U1",  "STM32F411CEU6", "UFQFPN-48", 25.40, 38.10, 0,   "top"),
    ("U2",  "AMS1117-3.3",   "SOT-223",   12.70, 10.16, 90,  "top"),
    ("Y1",  "8MHz",          "3215",       22.86, 35.56, 0,   "top"),
    ("R1",  "10k",           "0402",       15.24, 30.48, 0,   "top"),
    ("R2",  "10k",           "0402",       15.24, 28.44, 0,   "top"),
    ("C1",  "100nF",         "0402",       27.94, 40.64, 90,  "top"),
    ("C2",  "100nF",         "0402",       22.86, 40.64, 90,  "top"),
    ("C16", "10uF",          "0805",       10.16, 12.70, 0,   "top"),
    ("J1",  "USB-C",         "USB-C",      5.08,  25.40, 270, "top"),
]

print("Designator,Val,Package,Mid X,Mid Y,Rotation,Layer")
for row in pnp_data:
    print(f"{row[0]},{row[1]},{row[2]},{row[3]:.2f}mm,{row[4]:.2f}mm,{row[5]},{row[6]}")

print(f"\nTotal placements: {len(pnp_data)}")
print("Note: Verify rotation matches your EDA tool's convention")
print("JLCPCB uses 0° = component as shown in datasheet")

Designator,Val,Package,Mid X,Mid Y,Rotation,Layer
U1,STM32F411CEU6,UFQFPN-48,25.40mm,38.10mm,0,top
U2,AMS1117-3.3,SOT-223,12.70mm,10.16mm,90,top
Y1,8MHz,3215,22.86mm,35.56mm,0,top
R1,10k,0402,15.24mm,30.48mm,0,top
R2,10k,0402,15.24mm,28.44mm,0,top
C1,100nF,0402,27.94mm,40.64mm,90,top
C2,100nF,0402,22.86mm,40.64mm,90,top
C16,10uF,0805,10.16mm,12.70mm,0,top
J1,USB-C,USB-C,5.08mm,25.40mm,270,top

Total placements: 9
Note: Verify rotation matches your EDA tool's convention
JLCPCB uses 0° = component as shown in datasheet

Manufacturing Package Tool

Generate a manufacturing package checklist documenting all output files, specifications, and notes for your fabricator.

Exercises

Conclusion & Next Steps

You now know how to generate, verify, and organize every manufacturing output file your fabricator needs. From Gerber layers to drill files, BOM to pick-and-place data — a well-prepared manufacturing package means fewer questions, faster turnaround, and boards that match your design.