Understanding Excellon Drill File Format: Complete Technical Guide

The Excellon drill file format remains the de facto industry standard for PCB drilling data despite being developed in the 1980s. Every PCB designer eventually encounters these files, yet many struggle to understand what the cryptic commands and coordinate strings actually mean. After years of debugging drill file issues across dozens of projects, I have found that understanding the format structure saves countless hours of troubleshooting alignment problems, missing holes, and manufacturer rejections.

This guide breaks down the Excellon format in practical terms that working engineers can apply immediately when reviewing, editing, or troubleshooting drill files.

What Is Excellon Drill File Format

Excellon format is a text-based file format designed to drive CNC drilling and routing machines. The format originated from Excellon Automation, which dominated the PCB drilling equipment market during the 1980s. Their proprietary format became so widely adopted that it evolved into an industry standard used by virtually every PCB design tool and manufacturer today.

The format is technically a subset of RS-274D, the same specification family that Gerber format derives from. This shared heritage explains why drill files and Gerber files work together seamlessly in most CAM software.

Why Excellon Format Persists

Advantage	Description
Universal Support	Works on almost any PCB drilling machine
Proven Reliability	Decades of refinement and widespread use
Simplicity	Plain text format readable by humans
Open Standard	No licensing fees or proprietary restrictions
Software Support	Generated by all major PCB design tools

Despite newer formats like IPC-2581 and ODB++ offering richer data, Excellon remains dominant because it does one job exceptionally well and enjoys universal equipment support.

Excellon File Structure Overview

An Excellon drill file consists of ASCII text organized into distinct sections. Understanding this structure makes reading and editing files straightforward.

Basic File Organization

Section	Purpose	Required
Header	Global parameters and metadata	Recommended
Tool Definitions	Drill bit sizes and assignments	Essential
Drilling Commands	Hole coordinates and operations	Essential
Footer	Program termination	Required

The file reads top to bottom, with each command on its own line. The drilling machine processes commands sequentially, executing each instruction in order.

Sample Excellon File

A minimal but complete Excellon file looks like this:

M48METRIC,LZT01C0.80T02C1.00T03C3.20%T01X5250Y3100X5250Y4100X6750Y3100T02X8000Y5000X9500Y5000T03X2500Y2500M30

This file defines three tools, selects each tool in sequence, drills holes at specified coordinates, and terminates the program.

Header Section Commands

The header section begins with M48 and ends with either M95 or the percent sign (%). This section establishes global parameters that apply throughout the drilling operation.

Essential Header Commands

Command	Function	Example
M48	Start of header	M48
METRIC	Set metric units (mm)	METRIC
INCH	Set imperial units	INCH
M71	Set metric units (alternate)	M71
M72	Set imperial units (alternate)	M72
FMAT,1	Excellon Format 1 (drill only)	FMAT,1
FMAT,2	Excellon Format 2 (drill + route)	FMAT,2
M95	End of header	M95
%	End of header (alternate)	%

The unit declaration is critical because it affects how all subsequent coordinates are interpreted. Mismatched units between the header declaration and the actual coordinate data cause scaling errors by a factor of 25.4.

Zero Suppression Commands

Command	Meaning	Effect on Coordinates
LZ	Leading zeros	Leading zeros present, trailing suppressed
TZ	Trailing zeros	Trailing zeros present, leading suppressed
INCH,LZ	Inches with leading zeros	X001234 means X=1.234
METRIC,TZ	Metric with trailing zeros	X001234 means X=12.34

Zero suppression determines how the machine interprets coordinate values that lack explicit decimal points. This single setting causes more compatibility problems than any other aspect of the Excellon format.

Tool Definition Section

Tool definitions specify the drill bit diameters associated with each tool number. These definitions appear in the header section and must precede any drilling commands.

Tool Definition Syntax

The basic tool definition format is:

TnnCx.xxx

Where:

• T indicates a tool definition
• nn is the tool number (01-99)
• C indicates diameter follows
• x.xxx is the drill diameter in current units

Tool Definition Examples

Definition	Meaning
T01C0.80	Tool 1 = 0.80mm drill
T02C1.00	Tool 2 = 1.00mm drill
T03C0.0315	Tool 3 = 0.0315 inch (0.8mm) drill
T1C.04F300S55	Tool 1 = 0.04 inch, 300 IPM feed, 55000 RPM

Extended tool definitions may include feed rate (F) and spindle speed (S) parameters. These machine control parameters are important for CNC operators but do not affect the drill data itself.

Missing Tool Definitions Problem

Some older PCB design tools export drill files without embedded tool definitions:

M48T01F00S00T02F00S00T03F00S00%T01X01474Y02177

This file lacks the critical C parameter specifying drill diameters. Without tool sizes, manufacturers must guess or request additional information. Always verify your drill files include complete tool definitions before submitting for manufacturing.

Coordinate Format and Interpretation

Coordinate interpretation is the most confusing aspect of Excellon format. The format specification allows considerable flexibility, which creates ambiguity when reading files from different sources.

Coordinate Format Notation

Coordinate format is expressed as n:m where:

• n = digits before decimal point (integer portion)
• m = digits after decimal point (decimal portion)

Format	Units	Resolution	Max Value
2:3	Inches	0.001 inch	99.999 inches
2:4	Inches	0.0001 inch	99.9999 inches
2:5	Inches	0.00001 inch	99.99999 inches
3:3	Metric	0.001 mm	999.999 mm
4:2	Metric	0.01 mm	9999.99 mm

The 2:4 format is standard for inch units, while 3:3 is common for metric. Your PCB design software typically selects appropriate formats automatically.

Interpreting Coordinates with Zero Suppression

The interaction between coordinate format and zero suppression determines actual hole positions:

Raw Coordinate	Format	Zero Suppression	Actual Position
X1234Y5678	2:4	Leading (LZ)	X=0.1234, Y=0.5678
X1234Y5678	2:4	Trailing (TZ)	X=12.34, Y=56.78
X001234Y005678	2:4	None	X=0.1234, Y=0.5678
X123400Y567800	2:4	None	X=12.34, Y=56.78

The same raw coordinate string produces vastly different results depending on zero suppression settings. This ambiguity explains why Gerber viewers sometimes display drill holes in wrong positions.

Explicit Decimal Points

Modern Excellon files often include explicit decimal points, eliminating ambiguity:

X1.234Y5.678

When coordinates include decimal points, the values are interpreted literally regardless of zero suppression settings. This approach is more reliable but increases file size slightly.

Drilling Commands

After the header and tool definitions, the body section contains the actual drilling instructions.

Basic Drilling Operations

Command	Function
Tnn	Select tool number nn
XnnnYnnn	Drill hole at coordinates
G00XnnnYnnn	Rapid move to coordinates (no drill)
G05	Enable drill mode
M30	End of program

Tool selection (Tnn) tells the machine which drill bit to use. All subsequent XY coordinates use that tool until another tool selection appears.

Coordinate Commands

The most common command is simply XY coordinates without any prefix:

T01X5250Y3100X5250Y4100X6750Y3100

This sequence selects tool 1, then drills three holes at the specified locations. The machine assumes drill mode unless routing commands appear.

Routing Commands

Excellon Format 2 (FMAT,2) supports routing operations for creating slots and cutouts:

Command	Function
G00	Rapid positioning (move without cutting)
G01	Linear interpolation (straight line routing)
G02	Clockwise arc routing
G03	Counterclockwise arc routing
G85	Slot drilling (drill series of holes)
M15	Plunge router down
M16	Lift router up

Routing commands enable complex slot shapes that simple drilling cannot achieve.

Excellon Format 1 vs Format 2

Two major Excellon format versions exist, reflecting the evolution of drilling equipment capabilities.

Format Comparison

Feature	Format 1 (FMAT,1)	Format 2 (FMAT,2)
Drilling	Supported	Supported
Routing	Not supported	Supported
Slot commands	Limited	Full G85 support
Arc interpolation	Not supported	G02/G03 supported
Typical use	Legacy systems	Modern systems

Format 1 handles drilling operations only and remains compatible with older equipment. Format 2 adds routing capabilities required for slot holes and complex board outlines.

Most modern PCB design software defaults to Format 2, but many manufacturers accept either format for simple drilling applications.

Common Excellon File Problems

Understanding common problems helps you identify and fix issues quickly.

Missing or Incomplete Headers

Problem	Symptom	Solution
No M48	Parser confusion	Add M48 at file start
No unit declaration	Scale errors	Add METRIC or INCH
No tool sizes	Unknown hole diameters	Add TnnCx.xxx definitions
No header terminator	Parser errors	Add % or M95

Files missing critical header information force manufacturers to guess parameters, introducing errors.

Zero Suppression Mismatches

When a viewer or CAM system interprets zero suppression differently than intended:

Symptom	Likely Cause
Holes clustered in corner	Wrong zero suppression
Holes scaled 10x or 0.1x	Unit mismatch
Holes offset from pads	Format digits wrong

Adjusting the viewer’s import settings usually resolves these display issues without modifying the actual file.

Tool Definition Errors

Error Type	Example	Problem
Missing diameter	T01F00S00	No C parameter
Wrong units	T01C0.80 with INCH	0.80 inch vs 0.80mm
Duplicate tools	T01C0.80 and T01C1.00	Conflicting definitions

Verifying Excellon Files

Always verify drill files before submitting for manufacturing.

Verification Methods

Method	Tools	What to Check
Visual overlay	Gerbv, CAM350, ViewMate	Drill alignment with pads
Text inspection	Any text editor	Tool definitions present
Hole count	CAM software	Total matches design
Tool report	Gerber viewer	Sizes match requirements

Opening the file in a text editor provides quick verification that essential elements exist. Visual overlay with copper layers confirms alignment.

Recommended Viewers

Viewer	Platform	Features
Gerbv	Cross-platform	Free, open source
FlatCAM	Cross-platform	CNC output capability
CAM350	Windows	Industry standard
ViewMate	Windows	Professional features
GerberLogix	Windows	Quick verification

Useful Resources

Specifications and Documentation

Resource	Description
XNC Specification (Ucamco)	Free, unambiguous subset specification
IPC-NC-349	Official IPC drill format standard
Wikipedia PCB NC Formats	Overview of NC format variants

Software Tools

Tool	URL	Purpose
Gerbv	gerbv.github.io	Free Gerber/drill viewer
FlatCAM	flatcam.org	CAD/CAM for CNC milling
Online Gerber Viewer	gerber-viewer.easyeda.com	Quick web-based verification

Manufacturer Guidelines

Manufacturer	Resource
JLCPCB	jlcpcb.com/help (drill file troubleshooting)
Eurocircuits	eurocircuits.com (format documentation)
PCB Prime	pcbprime.com/pcb-tips/drill-file

Frequently Asked Questions

What is the difference between Excellon 1 and Excellon 2 format?

Excellon 1 (FMAT,1) supports drilling operations only and was designed for early CNC drilling machines. Excellon 2 (FMAT,2) adds routing capabilities including linear interpolation, arc commands, and slot drilling. Format 2 enables creation of complex slots and cutouts that simple drilling cannot achieve. Most modern equipment supports both formats, but Format 2 is standard for new designs. If your file contains routing commands (G01, G02, G03, G85), you need Format 2 compatibility.

Why do my drill holes appear offset from the copper pads?

Offset drill holes typically result from zero suppression mismatch between the drill file settings and your viewer’s interpretation. If the file specifies leading zero suppression but the viewer assumes trailing zeros (or vice versa), coordinates are interpreted incorrectly. Check the file header for LZ or TZ declarations and configure your viewer to match. Also verify that both Gerber and drill files use the same unit system (INCH or METRIC) and coordinate format.

How do I add missing tool definitions to an Excellon file?

Open both the drill file and the tool report (if separate) in a text editor. For each tool, create a definition line in the format TnnCx.xxx where nn is the tool number and x.xxx is the diameter. Insert these definitions between M48 and the percent sign (%). Ensure the diameter units match the file’s unit declaration. For example, if the file uses METRIC, a 0.8mm drill becomes T01C0.80. Save the file and verify in a Gerber viewer.

What coordinate format should I use for manufacturing?

Most manufacturers accept either 2:4 format for inches or 3:3 format for metric units. These provide sufficient precision for standard PCB manufacturing. The 2:4 format offers 0.0001 inch (0.1 mil) resolution, while 3:3 provides 0.001mm resolution. Always match your drill file format to your Gerber file format to ensure alignment. When in doubt, check your manufacturer’s documentation or use explicit decimal points in coordinates to eliminate ambiguity.

Can I convert between Excellon and Gerber formats?

Yes, several CAM tools can convert Excellon drill files to Gerber format and vice versa. FlatCAM, CAM350, and various online converters support this conversion. However, conversion may lose some information since Gerber and Excellon serve different purposes. Gerber describes images while Excellon describes drilling operations. For manufacturing, keeping files in their native formats typically produces better results than conversion.

Best Practices for Reliable Drill Files

Following consistent practices prevents the most common problems.

During Design

Configure your PCB design software to embed complete tool definitions in the header. Enable explicit unit declarations (METRIC or INCH) rather than relying on defaults. Use coordinate formats appropriate for your board size and precision requirements.

During Export

Verify export settings match your manufacturer’s requirements before generating files. Export drill and Gerber files together using the same origin point and unit system. Include clear file naming that identifies the file contents.

Before Submission

Open drill files in a text editor to verify headers contain unit declarations and tool definitions. Load both Gerber and drill files in a viewer to confirm visual alignment. Count total holes and verify against your design. Package all files in a single archive for submission.

Understanding Excellon drill file format transforms mysterious manufacturing problems into straightforward debugging tasks. The format’s simplicity, once understood, makes it reliable and predictable across virtually any PCB manufacturing workflow.