How to Export Gerber, Drill Files, BOM, and Pick-and-Place Files in KiCad 9.0

Generating manufacturing-ready output files is the critical final step in any PCB design workflow. KiCad 9.0 provides a streamlined process for exporting Gerber files, drill files, Bill of Materials (BOM), and pick-and-place files—the four essential deliverables required by PCB fabrication and assembly houses. This guide walks you through each export procedure with the correct settings to ensure error-free manufacturing.

Understanding Manufacturing Output Files

Before diving into the export procedures, it’s worth understanding what each file type communicates to your manufacturer.

Gerber files use the RS-274X format to describe each copper layer, solder mask, silkscreen, and board outline as 2D vector images. These files are the industry standard and contain no proprietary design data—only the graphical information needed to fabricate each layer.

Drill files (Excellon format) specify hole positions, diameters, and types (plated through-hole vs. non-plated). Without accurate drill files, your vias, mounting holes, and component through-holes cannot be manufactured correctly.

BOM files list every component on your board with reference designators, values, footprints, and manufacturer part numbers. Assembly houses use this to source and verify components.

Pick-and-place files (also called centroid or XY files) provide the exact coordinates and rotation angles for each surface-mount component. Automated pick-and-place machines read these files to position components on the PCB during assembly.

Prerequisites Before Export

Running a Design Rule Check (DRC) before generating any output files is strongly recommended. DRC identifies clearance violations, unconnected nets, and other errors that could cause manufacturing defects or electrical failures. In the PCB Editor, access this through Inspect → Design Rules Checker. Resolve all errors and review warnings before proceeding.

Additionally, ensure your zone fills are current. Outdated copper pours can result in incorrect Gerber output. Use Edit → Fill All Zones or press B to refresh all zones.

Exporting Gerber Files in KiCad 9.0

Open your design in the PCB Editor (the layout view, not the schematic). Navigate to File → Plot to access the Gerber generation dialog.

Layer Selection

From the top menu, go to: File → Plot

Select all layers required for your board. A typical two-layer board requires:

• F.Cu – Front copper layer
• B.Cu – Back copper layer
• F.Paste – Front solder paste (for stencil generation)
• B.Paste – Back solder paste
• F.SilkS – Front silkscreen
• B.SilkS – Back silkscreen
• F.Mask – Front solder mask
• B.Mask – Back solder mask
• Edge.Cuts – Board outline

For multilayer boards, include all internal copper layers (In1.Cu, In2.Cu, etc.).

Recommended Plot Settings

Configure the following options for reliable manufacturing output:

• Plot format: Gerber
• Output directory: Specify a dedicated folder (e.g., ./gerber/)
• Use Protel filename extensions: Enable this for broader compatibility with manufacturer systems
• Generate Gerber job file: Recommended for automated processing
• Subtract soldermask from silkscreen: Prevents silkscreen printing over exposed pads
• Check zone fills before plotting: Enables automatic zone refill verification
• Use drill/place file origin: Maintains coordinate consistency across all output files

Under Gerber Options, ensure:

• Coordinate format: 4.6 (unit mm) provides sufficient precision
• Use extended X2 format: Enable for modern Gerber features (most fabs support this)
• Include netlist attributes: Useful for automated inspection systems

Click Plot to generate the Gerber files. If KiCad detects outdated zone fills, select Refill when prompted.

Exporting Drill Files

Drill file generation is accessed from the same Plot dialog. Click Generate Drill Files… in the lower-right corner.

Drill File Settings

Configure these parameters:

• Drill file format: Excellon
• Drill units: Millimeters (or inches, matching your design units)
• Zeros format: Decimal format is universally supported
• Map file format: PostScript, PDF, or Gerber X2 (optional, for visual verification)
• Drill origin: Use drill/place file origin for coordinate consistency

PTH and NPTH Separation

Enable Merge PTH and NPTH holes into one file only if your manufacturer explicitly accepts combined files. Most fabricators prefer separate files distinguishing plated through-holes from non-plated holes, as they require different processing steps.

Click Generate Drill File to create the Excellon output. If your design includes blind or buried vias, KiCad generates separate drill files for each layer span.

Exporting the Bill of Materials

BOM generation occurs in the Schematic Editor, not the PCB Editor. Open your schematic and navigate to Tools → Generate BOM.

Configuring BOM Output

KiCad 9.0 provides built-in BOM export without requiring external plugins. In the BOM dialog:

• Format: Select CSV for universal compatibility, or Excel format for direct spreadsheet use
• Fields: Include Reference, Value, Footprint, Quantity, and any custom fields (e.g., MPN, Manufacturer, Supplier)
• Group components by: Value and Footprint (combines identical components into single line items)

Ensure your schematic symbols contain complete attribute data. Missing manufacturer part numbers or incorrect values will propagate to your BOM, potentially causing sourcing errors during assembly.

Click Export and specify your output filename. Review the generated file to verify all components are captured with accurate specifications.

Exporting Pick-and-Place Files

Return to the PCB Editor for component placement data. Access the export through File → Fabrication Outputs → Component Placement (.pos).

Position File Settings

Configure the following:

• Format: CSV (ASCII format compatible with most SMT lines)
• Units: Millimeters (standard for modern equipment)
• Files: Generate separate files for top and bottom sides, or a single unified file
• Use drill/place file origin: Must match your Gerber and drill file origin

The generated file contains columns for reference designator, value, package, X position, Y position, rotation, and side (top/bottom). Assembly houses use this data to program pick-and-place machines for automated component mounting.

Verifying Placement Data

Cross-reference the pick-and-place file against your layout. Incorrect rotation values are a common issue—components may be defined with different zero-rotation orientations in various footprint libraries. Many assembly houses provide DFM (Design for Manufacturability) review services that catch such discrepancies before production.

Organizing Your Manufacturing Package

A complete manufacturing package should include:

• All Gerber layers (.gbr or .gtl/.gbl/.gts/.gbs/.gto/.gbo extensions)
• Drill files (.drl or .xln)
• Drill map (optional, for visual reference)
• BOM file (.csv or .xlsx)
• Pick-and-place file (.pos or .csv)
• Gerber job file (.gbrjob, if generated)
• Assembly drawings or layer stackup documentation (if applicable)

Compress these files into a single ZIP archive for submission. Most PCB manufacturers provide online Gerber viewers—use these tools to visually verify your files before placing an order.

Troubleshooting Common Export Issues

Missing board outline: Ensure Edge.Cuts layer contains a closed polygon defining your board perimeter. Open contours or overlapping segments cause import failures.

Misaligned drill holes: Verify you’re using consistent origin settings across all exports. The drill/place file origin should match between Gerber, drill, and pick-and-place generation.

Empty BOM output: Check that your schematic symbols have populated value fields and are annotated (unique reference designators assigned).

Incorrect component rotation: Footprint orientation conventions vary by library. Compare your pick-and-place rotation values against datasheet land patterns.

Conclusion

Exporting manufacturing files in KiCad 9.0 follows a logical workflow: Gerbers and drill files from the PCB Editor, BOM from the Schematic Editor, and pick-and-place from fabrication outputs. By using consistent coordinate origins, verifying your design rules before export, and organizing files clearly for your manufacturer, you minimize the risk of fabrication errors and assembly defects. With these procedures established, you can confidently transition your KiCad designs from digital layout to physical hardware.