How to Generate NC Drill Files in KiCad: Complete PCB Engineer’s Guide

KiCad has become my go-to PCB design tool for both personal projects and professional work. It’s free, open-source, and genuinely capable of handling complex multilayer designs. But here’s something I’ve noticed after helping dozens of engineers transition to KiCad: the drill file generation process trips people up more than it should.

This guide walks you through everything you need to know about generating NC drill files in KiCad, from basic exports to handling tricky scenarios like oval holes and PTH/NPTH separation.

Understanding NC Drill Files and the Excellon Format

Before diving into KiCad’s interface, let’s establish what we’re actually creating. NC drill files (Numerical Control drill files) contain the precise instructions that CNC drilling machines need to place every hole in your PCB. The coordinates, tool sizes, and drilling sequences are all encoded in these files.

KiCad exports drill data in Excellon format, which is the industry standard accepted by virtually every PCB fabricator worldwide. You’ll sometimes hear this called “NC drill” or simply “drill files” — they’re all referring to the same thing.

What Information NC Drill Files Contain

Data Element	Description	Example
Tool Table	Drill bit diameters used	T1C0.300 (0.3mm drill)
X,Y Coordinates	Position of each hole	X015000Y025000
Tool Selection	Which drill to use	T01
Units Header	Metric or Imperial	METRIC,LZ
Format Info	Coordinate precision	FMAT,2

Pre-Export Checklist: Before Generating NC Drill Files

Running through this checklist before exporting has saved me countless headaches over the years.

Run Design Rule Check (DRC)

Always run DRC before generating any fabrication outputs. In KiCad’s PCB Editor:

Inspect → Design Rules Checker

Fix any errors related to:

• Minimum hole sizes
• Drill-to-copper clearances
• Via annular ring violations
• Overlapping holes

Verify Zone Fills Are Current

If your copper pours are outdated, KiCad will prompt you during export. Save yourself the interruption by refilling zones first:

Edit → Fill All Zones (or press B)

Check Your Board Origin

The drill origin setting determines the reference point for all hole coordinates. Inconsistent origins between Gerber and drill files cause the most common alignment problems I see from KiCad users.

Step-by-Step Guide: Generate NC Drill Files in KiCad

Step 1: Access the Plot Dialog

With your PCB design open in PCB Editor, navigate to:

File → Fabrication Outputs → Gerbers (.gbr)

This opens the Plot dialog. While primarily for Gerber generation, the drill file export is accessed from this same window.

Step 2: Open the Drill File Generator

At the bottom right of the Plot dialog, click:

Generate Drill Files…

This opens the dedicated drill file configuration dialog where you’ll set all the critical parameters.

Step 3: Configure Output Folder

The output folder defaults to the same location as your Gerber files, which is usually what you want. If you need a different location, click the folder icon to browse.

Recommended Practice: Keep all fabrication outputs (Gerbers and drill files) in the same folder for easier packaging when submitting to manufacturers.

Step 4: Configure Drill File Format Settings

This is where the critical decisions happen. Here are the recommended settings for most PCB fabricators:

Setting	Recommended Value	Notes
Drill File Format	Excellon	Industry standard
Mirror Y Axis	Unchecked	Leave unchecked unless specifically required
Minimal Header	Unchecked	Full header improves compatibility
PTH and NPTH in single file	Depends on manufacturer	See section below
Oval Holes Drill Mode	Use alternate drill mode	Better slot handling

Step 5: Configure Drill Units

Choose your coordinate units:

Option	When to Use
Millimeters	Metric designs, most international fabs
Inches	Imperial designs, some US-based fabs

Critical: Your drill file units should match your Gerber file units for best results.

Step 6: Set Drill Origin

The drill origin determines the coordinate reference point:

Option	Description	Recommendation
Absolute	Uses KiCad’s page origin (top-left)	Default, works for most cases
Drill/place file origin	Uses the auxiliary origin you set	Better for precise alignment

If you’ve set a drill/place origin on your board (using Place → Drill/Place File Origin), select “Drill/place file origin” here for consistent alignment with your Gerber files.

Step 7: Configure Zeros Format

Zero suppression affects file size and compatibility:

Format	Description	Recommendation
Decimal format	Full decimal notation	Most compatible, recommended
Suppress leading zeros	Removes leading zeros	Common alternative
Suppress trailing zeros	Removes trailing zeros	Less common
Keep zeros	No suppression	Maximum compatibility

Decimal format is the safest choice and what most modern CAM systems expect.

Step 8: Generate the Drill Files

Click Generate Drill File to create your output files. KiCad will generate:

• Main drill file (.drl extension)
• Separate NPTH file if applicable (-NPTH.drl)
• Report file with hole summary

Watch the message area at the bottom of the dialog for confirmation that files were created successfully.

Understanding PTH vs. NPTH Drill Files

One of the most common questions I get about KiCad drill files concerns the PTH/NPTH separation.

What Are PTH and NPTH Holes?

Hole Type	Full Name	Description	Examples
PTH	Plated Through-Hole	Copper-plated barrel	Vias, through-hole component leads
NPTH	Non-Plated Through-Hole	No copper plating	Mounting holes, mechanical features

Separate Files vs. Merged Files

KiCad gives you the option to generate PTH and NPTH holes in separate files or merged into one:

“PTH and NPTH in single file” checkbox:

Setting	Result	When to Use
Checked	One combined .drl file	Fabs that prefer single file (OSH Park, etc.)
Unchecked	Separate .drl and -NPTH.drl files	Fabs that require separation (most professional fabs)

My Recommendation: Check your manufacturer’s requirements. When in doubt, keep them separate — fabs can always merge files, but they can’t always split them correctly.

Handling Oval Holes and Slots in KiCad

Oval holes (slots) require special handling in drill files because they’re not simple circular holes.

Oval Holes Drill Mode Options

Mode	How It Works	Compatibility
Use route command	G00 routing for oval holes	Best for complex slots
Use alternate drill mode	G85 command for slots	Good compatibility

The Use alternate drill mode setting generates slots using the G85 drilled slot command, which creates overlapping holes from start point to end point. This method has excellent compatibility with most fabricators.

Best Practices for Slots

1. Verify slot dimensions meet your fab’s minimum requirements
2. Check that slot end radii match available drill sizes
3. Include slot callouts in your fabrication notes
4. Verify slots appear correctly in your Gerber viewer

Generating Drill Map Files

Drill map files provide a visual representation of your drill data — extremely useful for verification and for manufacturers who want human-readable documentation.

Creating a Drill Map File

In the same Generate Drill Files dialog:

1. Select your preferred Map File Format:

Format	Description	Use Case
Gerber	Standard Gerber format	Best for Gerber viewers
PostScript	Vector graphics	Printing, documentation
PDF	Portable document	Easy viewing/sharing
SVG	Scalable vector	Web, documentation
DXF	AutoCAD format	CAD integration

1. Click Generate Map File

The map file shows drill locations with tool identifiers, making it easy to visually verify your drill data.

Verifying Your KiCad Drill Files

Never send drill files to manufacturing without verification. I’ve caught issues in verification that would have resulted in scrapped boards.

Using KiCad’s Built-in Gerber Viewer

KiCad includes GerbView, a capable Gerber and drill file viewer:

1. Open GerbView from KiCad’s main project window
2. File → Open Excellon Drill File(s)
3. Load your .drl file(s)
4. Load your Gerber files for comparison
5. Verify holes align with pads

External Verification Tools

Tool	Platform	Cost	Features
Gerbv	Windows/Linux	Free	Open source, reliable
ViewMate	Windows	Free version	Professional quality
Tracespace View	Web	Free	Browser-based
JLCPCB Viewer	Web	Free	Direct upload verification
PCBWay Viewer	Web	Free	Manufacturing preview

Verification Checklist

Before submitting to your manufacturer:

1. All holes visible and in correct positions
2. Holes centered on pads (no offset)
3. PTH holes appear on signal pads and vias
4. NPTH holes appear on mounting holes only
5. Slot positions and orientations correct
6. Drill report shows expected tool sizes
7. No missing holes or extra holes

Common NC Drill File Problems and Solutions

Problem 1: Drill Holes Offset from Pads

Symptoms: Holes appear shifted relative to copper pads in viewer

Causes and Solutions:

Cause	Solution
Mismatched origin settings	Use same origin for Gerber and drill export
Different units	Ensure both use same units (mm or inches)
Auxiliary origin not set	Set drill/place origin on board

Problem 2: Missing NPTH Holes

Symptoms: Mounting holes or mechanical features don’t appear

Solutions:

• Check “PTH and NPTH in single file” setting
• Verify holes are defined as NPTH in footprint
• Ensure -NPTH.drl file is included in your fab package

Problem 3: Oval Holes Appearing as Round

Symptoms: Slots render as circular holes

Solutions:

• Enable “Use alternate drill mode” for oval holes
• Verify pad properties show correct oval dimensions
• Check that hole shape is set to “Oval” not “Circular”

Problem 4: Holes Scaled Incorrectly

Symptoms: Entire drill pattern too large or too small

Solutions:

• Verify units match between Gerber and drill
• Check format settings (decimal vs. suppressed zeros)
• Ensure viewer is interpreting format correctly

Problem 5: Manufacturer Rejects Drill Files

Symptoms: Fab house reports format or compatibility issues

Solutions:

• Disable “Minimal header” option
• Use Decimal format for zeros
• Verify Excellon format is selected
• Check manufacturer’s specific requirements

KiCad Version Differences for Drill Export

KiCad’s drill export has evolved across versions. Here are the key differences:

Version	Notable Features
KiCad 5.x	Basic Excellon export, separate PTH/NPTH option
KiCad 6.x	Improved dialog, better format options
KiCad 7.x	Gerber X2 drill format option, refined UI
KiCad 8.x	Enhanced format support, IPC-2581 export
KiCad 9.x	Latest improvements, better defaults

If you’re using an older version, the general process remains similar, but some options may be in slightly different locations.

Best Practices for NC Drill File Management

File Naming Conventions

Use clear, descriptive names:

File	Suggested Name
PTH drill	ProjectName.drl or ProjectName-PTH.drl
NPTH drill	ProjectName-NPTH.drl
Drill map	ProjectName-drl_map.gbr
Drill report	ProjectName-drl_report.txt

Manufacturing Package Organization

ProjectName_Fabrication/├── ProjectName-F_Cu.gtl├── ProjectName-B_Cu.gbl├── ProjectName-F_Mask.gts├── ProjectName-B_Mask.gbs├── ProjectName-F_Silkscreen.gto├── ProjectName-B_Silkscreen.gbo├── ProjectName-Edge_Cuts.gm1├── ProjectName.drl├── ProjectName-NPTH.drl (if separate)├── ProjectName-drl_map.gbr (optional)└── README.txt (fab notes)

Version Control

Include your fabrication outputs in version control:

• Track changes to export settings
• Maintain history of sent-to-fab packages
• Enable rollback if issues discovered

Useful Resources for KiCad Users

Official Documentation

Resource	URL	Description
KiCad Documentation	kicad.org/docs	Official user manual
KiCad Forum	forum.kicad.info	Community support
KiCad GitLab	gitlab.com/kicad	Source and issues

Drill File Viewers

Tool	Access
Gerbv	gerbv.github.io
ViewMate	pentalogix.com
Tracespace	tracespace.io/view
Reference Gerber Viewer	gerber-viewer.ucamco.com

Manufacturer Guidelines

Most PCB manufacturers provide specific export guides for KiCad:

• JLCPCB: jlcpcb.com/help (search “KiCad”)
• PCBWay: pcbway.com/blog (KiCad tutorials)
• OSH Park: docs.oshpark.com/design-tools/kicad
• Eurocircuits: eurocircuits.com (design guidelines)

Frequently Asked Questions

What drill file format should I use in KiCad?

Use Excellon format with Decimal zeros format and Millimeters for units (unless your design is imperial). These settings provide the best compatibility with PCB manufacturers worldwide. Avoid minimal header unless specifically required, as the full header contains useful format information.

Should I merge PTH and NPTH holes into one file?

It depends on your manufacturer. Some fabs like OSH Park prefer a single merged file, while others require separate files for plated and non-plated holes. When in doubt, check your manufacturer’s guidelines or generate separate files — professional fabs can merge them if needed.

Why are my drill holes offset from the pads?

Drill-to-pad offset almost always results from mismatched origin settings between your Gerber and drill exports. Ensure both use the same origin (either Absolute or Drill/place file origin). Also verify that units match between both file types.

How do I export slots and oval holes correctly?

Enable “Use alternate drill mode” in the drill file generation dialog. This uses the G85 drilled slot command to create oval holes properly. Also verify that your pads have the correct oval dimensions defined in their properties.

Does KiCad support blind and buried vias in drill files?

Yes, KiCad supports blind and buried vias for multilayer designs. When you define via types in your layer stackup with specific start/end layers, KiCad automatically generates appropriate drill files for each layer pair. Make sure your via definitions are correct in the board setup before generating outputs.

KiCad NC Drill Export vs. Other PCB Tools

Having worked with multiple PCB design platforms, I can offer perspective on how KiCad’s drill export compares.

Feature Comparison Across Tools

Feature	KiCad	Altium	Eagle	OrCAD
Excellon Export	Yes	Yes	Yes	Yes
PTH/NPTH Separation	Option	Option	Manual	Option
Gerber X2 Drill	Yes (7.0+)	Yes	No	Yes
Built-in Viewer	GerbView	CAMtastic	Limited	Yes
Slot Support	G85	G85	Limited	G85
Cost	Free	$$$$	$$	$$$

KiCad’s Advantages for Drill Export

Simplicity: KiCad’s drill export is accessed from a single, well-organized dialog. No hunting through multiple menus.

Sensible Defaults: Recent KiCad versions ship with reasonable default settings that work for most manufacturers.

Community Support: The active KiCad community means manufacturer-specific export guides are readily available.

Continuous Improvement: Being open-source, KiCad’s export capabilities improve with each release based on user feedback.

Advanced Topics: Multilayer Boards and Via Types

Handling Blind and Buried Vias

For complex HDI designs, KiCad supports multiple via types that require separate drill operations:

Via Type	Layer Span	Drill File Behavior
Through-hole	Full stack	Main .drl file
Blind (top)	Top to inner	Separate drill file
Blind (bottom)	Inner to bottom	Separate drill file
Buried	Inner to inner	Separate drill file
Microvia	Adjacent layers	Laser drill file

When your design includes blind or buried vias, KiCad automatically generates separate drill files for each layer pair. Ensure your via types are properly defined in Board Setup → Board Stackup.

Back Drilling Considerations

For high-speed designs requiring back drilling (controlled depth drilling), you’ll need to coordinate with your manufacturer separately. KiCad’s standard drill export doesn’t include back drill specifications — these are typically handled through fabrication notes and drawings.

Automating Drill File Generation with KiBot

For production environments or repetitive projects, consider using KiBot — a command-line tool for automating KiCad outputs.

Basic KiBot Configuration for Drill Files

yaml

outputs:  – name: ‘drill_files’    type: ‘excellon’    options:      metric_units: true      pth_and_npth_single_file: false      use_aux_axis_as_origin: true      output: ‘%f-%i.%x’

Benefits of Automation

Benefit	Description
Consistency	Same settings every time
Speed	Generate all outputs with one command
CI/CD Integration	Automate in build pipelines
Error Reduction	No manual setting mistakes

KiBot is available at: github.com/INTI-CMNB/KiBot

Manufacturer-Specific Export Tips

Different fabricators have different preferences. Here are tips for popular services:

JLCPCB Settings

Setting	JLCPCB Preference
PTH/NPTH	Either (merged OK)
Units	Millimeters
Format	Decimal
Origin	Absolute

OSH Park Settings

Setting	OSH Park Preference
PTH/NPTH	Merged preferred
Format	2:4 or 3:3
Binary .DRL	Not recommended

PCBWay Settings

Setting	PCBWay Preference
PTH/NPTH	Separate files OK
Units	Either (specify in notes)
Slots	G85 command supported

Always check your specific manufacturer’s current guidelines, as requirements can change.

Conclusion: Reliable NC Drill File Generation in KiCad

Generating NC drill files in KiCad is straightforward once you understand the key settings and their implications. The most important principles to remember:

1. Run DRC before generating any fabrication outputs
2. Match settings between Gerber and drill exports (origin, units)
3. Use Excellon format with decimal zeros for best compatibility
4. Know your manufacturer’s requirements for PTH/NPTH separation
5. Always verify your outputs before sending to fabrication
6. Keep files organized with clear naming conventions

KiCad’s drill file generation has matured significantly over recent versions. What was once a common source of manufacturing issues has become a reliable, well-designed export process. Take the time to understand each setting, verify your outputs, and you’ll have no trouble getting your boards manufactured correctly.

The open-source nature of KiCad means the community continuously improves these features. If you encounter issues, the KiCad forum is an excellent resource where experienced users and developers actively help troubleshoot problems.