KiCad to JLCPCB, PCBWay & OSHPark: Export & Order Guide

Getting your KiCad design manufactured should be the exciting finish line of a project, not a frustrating exercise in file format troubleshooting. Yet the number of forum posts asking “why won’t JLCPCB accept my Gerbers?” or “what settings does PCBWay need?” suggests many designers struggle with this final step.

The reality is that each PCB manufacturer has slightly different preferences for Gerber settings, drill file formats, and assembly file requirements. What works perfectly for JLCPCB KiCad exports might cause issues at OSHPark or Eurocircuits. This guide covers the exact export settings for the most popular fabrication houses, from budget-friendly Chinese manufacturers to premium European and American options.

Whether you’re ordering bare boards from PCBWay KiCad projects or getting full assembly from JLCPCB, understanding these manufacturer-specific requirements saves time, money, and the frustration of rejected orders or incorrectly manufactured boards.

Pre-Export Checklist: KiCad DRC and Design Verification

Before generating any manufacturing files, running a thorough Design Rule Check prevents the majority of fabrication issues. The KiCad JLCPCB DRC process catches problems that would otherwise result in rejected orders or boards that don’t work.

Running DRC in KiCad

1. Open your PCB in the PCB Editor
2. Go to Inspect → Design Rules Checker (or press the DRC icon)
3. Click “Run DRC”
4. Fix all errors before proceeding
5. Review warnings individually (some may be acceptable)

Critical Pre-Export Steps

Step	Why It Matters
Run DRC	Catches clearance violations, unconnected nets
Refill zones (press B)	Ensures copper pours reflect current design
Check zone fills before plotting	KiCad prompts if zones are outdated
Update board from schematic	Syncs any last-minute changes
Verify mounting holes	Confirm NPTH vs PTH settings

Zone fills are particularly important. If you’ve made routing changes since the last zone fill, your Gerbers won’t match your intended design. KiCad can prompt you during export, but catching this earlier avoids confusion.

Understanding Gerber Files and What Manufacturers Need

Gerber files are the industry standard for PCB manufacturing data. Each layer of your design becomes a separate Gerber file, and together with drill files, they provide everything a manufacturer needs to fabricate your board.

Standard Two-Layer PCB File Set

File	KiCad Layer	Protel Extension	Purpose
Top Copper	F.Cu	.GTL	Front copper traces
Bottom Copper	B.Cu	.GBL	Back copper traces
Top Solder Mask	F.Mask	.GTS	Front mask openings
Bottom Solder Mask	B.Mask	.GBS	Back mask openings
Top Silkscreen	F.SilkS	.GTO	Front legend/text
Bottom Silkscreen	B.SilkS	.GBO	Back legend/text
Board Outline	Edge.Cuts	.GKO	PCB shape/boundary
Drill File	N/A	.DRL	Hole locations/sizes

For four-layer boards, add In1.Cu and In2.Cu to your export. Six-layer designs need In1.Cu through In4.Cu.

Protel vs KiCad Filename Extensions

Most manufacturers prefer Protel filename extensions (.GTL, .GBL, etc.) over KiCad’s default naming. The “Use Protel filename extensions” checkbox in the Plot dialog handles this automatically. While modern fab houses can usually identify KiCad’s native filenames, using Protel extensions reduces the chance of layer misidentification.

JLCPCB KiCad Export Settings

JLCPCB is arguably the most popular choice for hobbyist and prototype PCB manufacturing. Their JLCPCB KiCad documentation is comprehensive, but here are the exact settings that work reliably.

Gerber Settings for JLCPCB

Open File → Fabrication Outputs → Gerbers (.gbr) and configure:

Layer Selection (2-layer board):

• F.Cu, B.Cu
• F.Mask, B.Mask
• F.SilkS, B.SilkS
• Edge.Cuts
• F.Paste, B.Paste (if ordering stencils)

General Options:

• Plot footprint values: Unchecked
• Plot reference designators: Checked
• Check zone fills before plotting: Checked
• Use drill/place file origin: Checked

Gerber Options:

• Use Protel filename extensions: Checked
• Subtract soldermask from silkscreen: Checked
• Coordinate format: 4.6 (mm)

Drill File Settings for JLCPCB

Click “Generate Drill Files” in the Plot dialog:

Setting	Value
Drill File Format	Excellon
PTH and NPTH	Single file (or separate, both work)
Oval Holes Drill Mode	Use alternate drill mode
Drill Origin	Absolute
Drill Units	Millimeters
Zeros Format	Decimal format

JLCPCB Assembly Files (BOM and CPL)

For SMT assembly service, JLCPCB requires BOM and CPL (Component Placement List) files in specific formats.

BOM File Requirements:

• Comment (part description/value)
• Designator (C1, R1, U1, etc.)
• Footprint (package size)
• LCSC Part Number (optional but recommended)

CPL File Requirements:

• Designator
• Mid X, Mid Y coordinates
• Rotation
• Layer (Top/Bottom)

The easiest approach is using the kicad-jlcpcb-tools plugin (github.com/Bouni/kicad-jlcpcb-tools), which generates correctly formatted files with one click and includes LCSC part number lookup.

Manual CPL Generation:

1. Go to File → Fabrication Outputs → Footprint Position (.pos) File
2. Format: CSV
3. Units: Millimeters
4. Files: Separate files for front and back

Note that JLCPCB requires specific column headers. The plugin handles this, but manual files may need header renaming.

PCBWay KiCad Export Settings

PCBWay offers similar services to JLCPCB with slightly different preferences. The KiCad PCBWay workflow benefits from their dedicated plugin that automates the entire process.

Using the PCBWay Plugin for KiCad

PCBWay provides an official plugin (github.com/pcbway/PCBWay-Plug-in-for-Kicad) that exports files and opens their ordering page directly:

1. Install via Plugin and Content Manager
2. Click the PCBWay button in PCB Editor
3. Files are automatically generated and uploaded
4. Complete your order on the PCBWay website

Manual Gerber Export for PCBWay

If you prefer manual export, use these settings:

Gerber Options:

• Use Protel filename extensions: Checked
• Do NOT check “Use extended X2 format” (PCBWay historically has issues with X2)
• Coordinate format: 4.6

Drill Settings:

• Suppress leading zeros: Checked
• Minimal header: Checked
• Drill Units: Millimeters

Important PCBWay Note: Their documentation explicitly states not to use extended X2 format for Gerbers. While many modern manufacturers support X2, PCBWay’s CAM system works better with standard RS-274X format.

PCBWay Assembly Files

For assembly orders, PCBWay needs:

• BOM in CSV format
• Position file (Footprint Position output from KiCad)

The position file works directly from KiCad’s output without modification in most cases.

OSHPark KiCad Settings and Native File Upload

OSHPark stands out by accepting native .kicad_pcb files directly. This eliminates Gerber generation entirely for OSHPark KiCad users.

Direct KiCad Upload to OSHPark

Simply upload your .kicad_pcb file to oshpark.com. Their system:

• Processes the file using KiCad 9.x internally
• Generates Gerbers on their end
• Shows a preview for verification

Advantages:

• No Gerber generation needed
• Fewer opportunities for export errors
• Simpler workflow for beginners

Considerations:

• Zone fills must be up to date (OSHPark doesn’t refill zones)
• Custom fonts may render differently (embed fonts in KiCad 9+)
• Design rules from .kicad_pro aren’t included

Gerber Export for OSHPark

If you prefer uploading Gerbers (for verification or using older KiCad versions):

Critical Settings:

• Uncheck “Plot sheet reference on all layers” (causes board size detection issues)
• Check “Exclude PCB Edge from other layers”
• Use Protel filename extensions: Recommended but not required

Drill Settings:

• Excellon format
• Decimal format for zeros
• Millimeters or inches both work

OSHPark’s system is notably flexible with file formats and will detect KiCad-generated files automatically.

Aisler KiCad Integration (European Manufacturer)

Aisler KiCad integration is exceptionally smooth for European designers wanting local manufacturing. Like OSHPark, Aisler accepts native KiCad files.

Aisler Push for KiCad Plugin

The official plugin (github.com/AislerHQ/PushForKiCad) provides one-click ordering:

1. Install via Plugin and Content Manager
2. Click “Push Layout to Aisler”
3. Files upload directly to your Aisler project
4. Complete order on aisler.net

What the Plugin Exports:

• Gerber files in optimized format
• IPC-Netlist for smart testing
• BOM file with MPN matching (if configured)

Direct Upload Benefits

Aisler’s native file support means:

• No manual Gerber generation
• Automatic DFM checking
• Smart test coverage analysis
• Revision tracking across uploads

For assembly services, add MPN (Manufacturer Part Number) fields to schematic symbols. Aisler reads these directly for component sourcing.

Eurocircuits KiCad Settings (European Premium)

Eurocircuits KiCad support includes native file upload and comprehensive DRC guidelines. As a premium European manufacturer, they offer tight tolerances and excellent quality.

Native KiCad File Upload

Eurocircuits accepts .kicad_pcb files directly through their PCB Visualizer, which provides immediate DFM feedback before ordering.

Gerber Export for Eurocircuits

When using Gerbers, Eurocircuits recommends:

• Gerber X2 or X3 format (they fully support extended formats)
• Include Gerber Job file for layer identification
• Clear, descriptive filenames

Design Rule Values for Standard Service:

Parameter	Standard Value
Minimum track width	0.15mm
Minimum clearance	0.15mm
Minimum via diameter	0.45mm
Minimum via drill	0.20mm
Minimum annular ring	0.125mm

Eurocircuits provides downloadable DRC settings for various CAD packages, though KiCad requires manual entry in Board Setup → Design Rules.

AllPCB KiCad Export Considerations

AllPCB KiCad users should note some specific requirements, particularly for assembly services.

Assembly File Requirements

AllPCB requires additional layers for assembly:

• Fabrication layers with component designators
• BOM in XLSX format (not CSV)
• Position file with specific column formatting

Export Fabrication Layers: Check F.Fab and B.Fab in your Gerber export if using assembly services. These layers show component outlines and reference designators that help assembly staff.

Gerber Settings

Standard settings work for bare board orders:

• Use Protel filename extensions
• Excellon drill format
• Decimal zeros format

PCB Manufacturer Comparison Table

Manufacturer	Native KiCad	Plugin	Typical 2-Layer Price	Lead Time	Assembly
JLCPCB	No	Yes (community)	$2-5	3-7 days	Yes
PCBWay	No	Yes (official)	$5-10	3-7 days	Yes
OSHPark	Yes	No	$5/sq inch	12+ days	No
Aisler	Yes	Yes (official)	€12+	1-7 days	Yes
Eurocircuits	Yes	No	€30+	2-7 days	Yes
AllPCB	No	No	$5-15	3-7 days	Yes
NextPCB	No	No	$2-5	3-7 days	Yes

Prices are approximate for small prototype quantities and vary based on specifications.

KiCad Fabrication Plugins and Tools

Several plugins streamline the export process for specific manufacturers.

JLCPCB Tools Plugin

Repository: github.com/Bouni/kicad-jlcpcb-tools

Features:

• One-click Gerber + BOM + CPL generation
• LCSC part number database search
• Rotation correction management
• Stock checking integration

Installation:

1. Open Plugin and Content Manager
2. Search “JLCPCB”
3. Install and restart KiCad

PCBWay Fabrication Toolkit

Repository: github.com/pcbway/PCBWay-Fabrication-Toolkit-for-KiCad

Features:

• Direct ordering integration
• Automatic file formatting
• Assembly file generation

Aisler Push Plugin

Repository: github.com/AislerHQ/PushForKiCad

Features:

• One-click upload to Aisler
• Project revision tracking
• Local export option available

Verifying Gerber Files Before Ordering

Always verify your exported Gerbers before uploading. Catching errors at this stage is free; catching them after manufacturing is expensive.

Free Gerber Viewers

Tool	Platform	Notes
KiCad GerbView	Cross-platform	Built into KiCad
Gerbv	Linux/Windows	Lightweight, fast
Gerblook.org	Web	Quick online check
JLCPCB Gerber Viewer	Web	Shows what JLCPCB will manufacture
PCBWay Gerber Viewer	Web	Included in order process

Verification Checklist

Check	What to Look For
Layer alignment	All layers registered correctly
Drill holes	Present and correctly sized
Board outline	Closed path, correct dimensions
Silkscreen	No text on pads, readable size
Solder mask	Correct pad exposure
Copper connections	No unintended shorts/opens

Configuring KiCad DRC for Different Manufacturers

Each manufacturer has different minimum specifications. Setting up the correct KiCad JLCPCB DRC rules before starting your layout prevents costly redesigns.

Setting Design Rules in KiCad

Go to File → Board Setup → Design Rules to configure constraints:

Constraints Tab:

• Minimum clearance
• Minimum track width
• Minimum connection width
• Minimum annular ring

Pre-defined Sizes Tab:

• Track widths
• Via sizes
• Differential pair dimensions

Manufacturer-Specific DRC Settings

Parameter	JLCPCB	PCBWay	OSHPark	Eurocircuits
Min Track	0.127mm (5mil)	0.1mm (4mil)	0.152mm (6mil)	0.15mm
Min Space	0.127mm (5mil)	0.1mm (4mil)	0.152mm (6mil)	0.15mm
Min Via Hole	0.3mm	0.3mm	0.254mm (10mil)	0.2mm
Min Via Diameter	0.5mm	0.5mm	0.508mm (20mil)	0.45mm
Min Annular Ring	0.13mm	0.1mm	0.127mm	0.125mm

These represent standard service levels. Tighter tolerances are available at higher prices.

Creating Manufacturer Templates

Create separate KiCad project templates for each manufacturer:

1. Set up a new project with correct design rules
2. Configure the Plot dialog settings
3. Save as template via File → New Project from Template → Save Current Project as Template

This ensures consistent export settings across all projects targeting that manufacturer.

Common Export Problems and Solutions

Missing Drill Holes

Symptom: Manufacturer reports no drill file or missing holes Solution: Always click “Generate Drill Files” separately after plotting Gerbers. It’s a separate step that’s easy to forget.

Board Outline Not Detected

Symptom: Quote shows wrong dimensions or upload fails Solution:

• Ensure Edge.Cuts layer contains a closed path
• Check for small gaps in the outline
• Remove any non-outline elements from Edge.Cuts

Zone Fills Outdated

Symptom: Copper pours don’t match expected design Solution: Press B to refill zones before export, or enable “Check zone fills before plotting”

Component Rotation Issues (Assembly)

Symptom: Parts placed at wrong angles in assembly preview Solution: The kicad-jlcpcb-tools plugin includes rotation correction. For manual files, edit the rotation column in the CPL file.

Silkscreen on Pads

Symptom: Manufacturer removes silkscreen unexpectedly Solution: Enable “Subtract soldermask from silkscreen” in Gerber options

Useful Resources and Download Links

Official Manufacturer Documentation

Manufacturer	KiCad Export Guide
JLCPCB	jlcpcb.com/help/article/how-to-generate-gerber-and-drill-files-in-kicad-8
PCBWay	pcbway.com/blog/help_center/Generate_Gerber_file_from_Kicad.html
OSHPark	docs.oshpark.com/design-tools/kicad/
Aisler	aisler.net/partners/kicad
Eurocircuits	eurocircuits.com/blog/kicad-design-rules/

Plugin Repositories

Plugin	URL
JLCPCB Tools	github.com/Bouni/kicad-jlcpcb-tools
PCBWay Plugin	github.com/pcbway/PCBWay-Plug-in-for-Kicad
Aisler Push	github.com/AislerHQ/PushForKiCad
JLCPCB BOM Plugin	github.com/wokwi/kicad-jlcpcb-bom-plugin

Gerber Verification Tools

Tool	URL
Gerbv	gerbv.github.io
Gerblook	gerblook.org
Ucamco Gerber Viewer	gerber-viewer.ucamco.com

Frequently Asked Questions

Can I upload .kicad_pcb files directly to JLCPCB instead of Gerbers?

No, JLCPCB requires Gerber files. Unlike OSHPark and Aisler, JLCPCB’s system doesn’t process native KiCad files. Use the standard export process or the JLCPCB Tools plugin to generate the required files. The plugin automates everything and produces correctly formatted Gerbers, BOM, and CPL files.

Why does KiCad’s default Gerber export not work with PCBWay?

KiCad’s defaults are generally compatible, but PCBWay specifically recommends not using “Extended X2 format” for Gerbers. Their CAM system processes standard RS-274X format more reliably. Also ensure “Use Protel filename extensions” is checked for easier layer identification.

What’s the difference between JLCPCB’s BOM and CPL files?

The BOM (Bill of Materials) lists what components go on the board with values, footprints, and part numbers. The CPL (Component Placement List, also called centroid or pick-and-place file) specifies where each component goes with X/Y coordinates, rotation, and which side of the board. Both are required for assembly services.

Should I use Gerber X2 format or standard RS-274X?

For JLCPCB and most Asian manufacturers, standard RS-274X works most reliably. For Eurocircuits and some European fabs, Gerber X2/X3 provides additional metadata that improves DFM checking. When in doubt, RS-274X (don’t check “Use extended X2 format”) is the safer choice. OSHPark and Aisler handle either format well through their native file processing.

How do I fix component rotation errors in JLCPCB assembly preview?

JLCPCB’s system expects certain rotation conventions that may differ from KiCad’s output. The kicad-jlcpcb-tools plugin includes a rotation correction database that automatically adjusts common footprints. For manual correction, edit the Rotation column in your CPL file. The plugin also has a Rotation Manager where you can add custom corrections for footprints not in the database.

Streamlining Your KiCad Manufacturing Workflow

The key to smooth PCB ordering is establishing a consistent workflow. Once you’ve configured export settings for your preferred manufacturer, save them as part of your project template. The community plugins for JLCPCB and PCBWay dramatically reduce friction by handling all the formatting details automatically.

Recommended Workflow Steps

1. Design Phase: Use manufacturer DRC settings from the start
2. Pre-Export: Run DRC, refill zones, update from schematic
3. Export: Use plugin or manual settings for target manufacturer
4. Verify: Check Gerbers in GerbView or online viewer
5. Upload: Submit to manufacturer and verify preview
6. Review: Check manufacturer’s DFM feedback before confirming

Cost Optimization Tips

When ordering from multiple manufacturers, consider:

JLCPCB KiCad Projects: Best for high-volume prototypes with assembly needs. Their parts library is extensive, and basic boards start at $2.

PCBWay KiCad Orders: Similar pricing to JLCPCB with occasionally better options for special finishes like gold fingers or heavy copper.

OSHPark KiCad Designs: Premium purple boards, excellent for US-based designers wanting simpler ordering. Cost scales with board size rather than fixed minimum orders.

Aisler KiCad Users: Ideal for European designers. Local manufacturing means faster delivery without customs hassles.

Eurocircuits KiCad Projects: When quality and precision matter more than cost. Excellent for high-reliability applications.

For beginners, OSHPark and Aisler’s native KiCad file support eliminates the Gerber learning curve entirely. Upload your board file, verify the preview, and order. As you gain experience, the flexibility of Gerber exports lets you shop around between manufacturers for the best combination of price, quality, and turnaround time.

Remember that every manufacturer’s engineers want your order to succeed. When in doubt about settings, their support teams are generally responsive and helpful. But with the correct export settings from this guide, most orders should process without any manual intervention.