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

Cadence Allegro handles drill file generation differently than most other PCB design tools, and this catches many engineers off guard. The default output format in Allegro is not standard Excellon, which means manufacturers often reject drill files that appear to generate successfully. After years of working with Allegro across multiple versions, I have learned that the key to reliable drill file generation lies in configuring NC Parameters before touching the NC Drill dialog.

This guide covers the complete process of generating NC drill files in Cadence Allegro that manufacturers will accept without questions or rework requests.

Understanding How Allegro Handles Drill Data

Unlike Altium Designer or KiCad where drill file generation follows a straightforward path, Cadence Allegro takes a more modular approach. The software separates NC parameter configuration from the actual drill file generation, requiring you to visit multiple dialogs to produce manufacturer-ready output.

Allegro stores drill information based on padstack definitions. Every via and through-hole component in your design references a padstack that contains hole size, plating status, and layer span information. The NC Drill command extracts this data and formats it according to your parameter settings.

Key Components of Allegro Drill Output

Component	Purpose	File Extension
NC Drill File	Hole coordinates and tool table	.drl, .tap
NC Route File	Slot and cutout routing paths	.rou
Drill Legend	Visual representation for fab drawing	Placed in design
nc_param.txt	Parameter metadata file	.txt
Drill Statistics	Hole count summary	.dts

The .drl or .tap file is what manufacturers need for CNC drilling machines. The other files provide supporting information but are not directly read by drilling equipment.

Critical First Step: Configuring NC Parameters

Before generating any drill files in Allegro, you must configure the NC Parameters. This step is essential because Allegro’s default settings produce files that most manufacturers cannot use directly.

Access NC Parameters through Manufacture → NC → NC Parameters (in Allegro) or Export → NC Parameters (in OrCAD PCB Editor).

NC Parameters Dialog Settings

Parameter	Recommended Setting	Reason
Code	ASCII	Modern standard, better compatibility
Enhanced Excellon Format	Enabled	Creates proper header with tool definitions
Auto Tool Select	Enabled	Inserts tool codes in data section
Output Units	Match Gerber units	Prevents scaling misalignment
Format	2.4 (inches) or 3.3 (metric)	Industry standard precision
Zero Suppression	Leading	Most compatible option
Coordinates	Absolute	Easier verification
Separate Files for Plated/Non-plated	Enabled	Required by most manufacturers

The Enhanced Excellon Format setting deserves special attention. When disabled, Allegro generates a non-standard drill file format that many Gerber viewers and manufacturer systems cannot interpret correctly. Enable this option to produce files with proper M48 headers, tool definitions in TnnC.xxx format, and INCH/METRIC declarations.

Why Enhanced Excellon Format Matters

Standard Allegro drill output without Enhanced Excellon Format lacks critical header information:

Information	Without Enhanced Excellon	With Enhanced Excellon
File header	Missing or minimal	M48 to % complete header
Tool definitions	Separate file required	Embedded TnnC.xxx format
Unit declaration	Ambiguous	Explicit INCH or METRIC
Zero suppression	Undefined	LZ or TZ specified

Manufacturers receiving files without proper headers often guess at format settings, leading to scaled holes or misaligned positions.

Step-by-Step NC Drill File Generation in Allegro

With NC Parameters configured correctly, the actual drill file generation becomes straightforward.

Accessing the NC Drill Dialog

Navigate to Manufacture → NC → NC Drill in Allegro PCB Editor. In OrCAD PCB Editor, the path is Export → NC Drill.

The NC Drill dialog presents several options that control output file generation.

Configuring the NC Drill Dialog

Option	Description	Recommended Setting
Root File Name	Base filename for output	Design name or meaningful identifier
Auto Tool Select	Insert tool codes in drill data	Enable
Drilling Output	Layer Pair or By Layer	Layer Pair for standard designs
Include Backdrill	Generate backdrill files	Enable if design uses backdrilling
Include Counterdrill	Include counterbore/countersink	Enable if design uses these features
Optimize Drill Head Travel	Reorder holes for efficiency	Optional, manufacturer may re-optimize

Generating the Drill Files

Click the Parameters button to verify NC Parameters settings one more time. Close the Parameters dialog, then click the Drill button.

Allegro generates drill files in your design directory. The filename follows the pattern: designname-l1-l2.drl where l1 and l2 indicate the layer span.

For designs with separate plated and non-plated holes, you will see additional files with “-np-” in the filename indicating non-plated holes.

Working with Blind and Buried Vias

Multilayer designs with blind or buried vias require special attention during drill file generation. Each unique layer pair that contains drilled holes generates its own drill file.

Layer Pair vs By Layer Output

Option	Use Case	Output Files
Layer Pair	Standard through-hole and stacked blind vias	One file per unique layer pair
By Layer	Microvia technology, sequential lamination	Separate file for each layer transition

For a six-layer board with blind vias from L1-L2 and L5-L6, plus buried vias from L2-L5 and through-holes from L1-L6, Layer Pair output generates four separate drill files.

Naming Convention for Multiple Drill Files

Layer Span	Plated Filename	Non-Plated Filename
L1 to L6 (through)	designname-1-6.drl	designname-np-1-6.drl
L1 to L2 (blind top)	designname-1-2.drl	designname-np-1-2.drl
L5 to L6 (blind bottom)	designname-5-6.drl	designname-np-5-6.drl
L2 to L5 (buried)	designname-2-5.drl	designname-np-2-5.drl

Provide all drill files to your manufacturer along with clear documentation about which file corresponds to which layer pair.

Creating the Drill Legend and Drill Table

A drill legend provides visual reference for hole sizes on your fabrication drawing. Allegro separates drill legend creation from drill file generation.

Generating the Drill Legend

Navigate to Manufacture → NC → Drill Legend in Allegro or Manufacture → Create Drill Table in OrCAD.

The Drill Legend dialog offers several customization options:

Option	Description
Template File	Controls legend appearance
Legend Title	Text appearing above the legend
By Hole Size	Sort order for hole listing
Include Backdrill	Show backdrill information
Non-plated First	List non-plated holes before plated

Click OK and the legend attaches to your cursor. Place it in a clear area of your fabrication drawing layer.

For designs with blind or buried vias, multiple drill legends generate and stack on top of each other. Use Edit → Move with Groups selected in the Find pane to separate them.

Customizing Drill Legend Content

Access Manufacture → NC → Drill Customization to modify drill table appearance before generation. This dialog allows changes to:

Setting	Purpose
Character types	Font selection
Character sizes	Text height
Drill tolerance	Displayed tolerance values
Column visibility	Show/hide specific columns

Verifying Drill Files Before Manufacturing

Never send drill files to manufacturing without verification. Allegro-generated files require checking to ensure they align correctly with Gerber layers and contain accurate hole information.

Recommended Gerber Viewers

Viewer	Platform	Key Features
GC-Prevue	Windows	Professional tool, excellent format support
Gerbv	Windows, Linux, macOS	Free, open source
ViewMate	Windows	Industry standard, free version available
CAM350	Windows	Professional CAM software
ZofzPCB	Windows	3D visualization

Load your Gerber files first, then add the drill file. Enable layer transparency and zoom into pad locations to verify alignment.

Verification Checklist

Check	What to Look For
Hole centering	All drill hits centered on pads
Scale	No 10x or 0.1x scaling errors
Hole count	Total matches design
Tool table	Correct sizes listed
Layer alignment	No systematic offset
Plating separation	PTH and NPTH in correct files

Scale errors of exactly 10x or 2.54x (metric/imperial confusion) indicate format mismatch between Gerber and drill settings.

Common Allegro Drill File Problems and Solutions

Years of experience with Allegro have revealed recurring issues that frustrate engineers and delay manufacturing.

Problem: Drill Holes Offset from Pads

This almost always traces back to mismatched settings between Gerber artwork and NC drill output.

Parameter	Check In Gerber	Check In NC Drill
Units	General Parameters → Output Unit	NC Parameters → Output Units
Format	General Parameters → Format	NC Parameters → Format
Zero Suppression	Film Control settings	NC Parameters → Zero Suppression
Coordinates	Usually Absolute	NC Parameters → Coordinates

Both dialogs must use identical values for alignment.

Problem: Manufacturer Cannot Read Drill File

The Enhanced Excellon Format option is probably disabled. Access NC Parameters and enable this setting, then regenerate drill files.

Also verify that Auto Tool Select is enabled. Without this option, tool codes may not appear in the drill data section where equipment expects them.

Problem: Missing Slot or Cutout Data

NC Drill only generates circular hole data. For slots, oblong holes, and board cutouts, you need NC Route output.

Navigate to Manufacture → NC → NC Route (Allegro) or Export → NC Route (OrCAD) to generate routing data. Both drill and route files are required for complete manufacturing data.

Problem: Holes Appearing as Dots in Gerber Viewer

Some viewers require external tool table files to display drill sizes. Allegro generates an nc_tools_auto.txt file containing tool definitions. If your viewer cannot read the embedded tool table, import this file manually.

Also check that you selected Enhanced Excellon Format, which embeds tool sizes in the TnnC.xxx format within the drill file header.

Problem: Wrong Number of Drill Files Generated

For blind and buried via designs, Allegro generates separate files for each layer pair. If you expected one file but received multiple, your design likely contains vias that span different layer combinations.

Review your via definitions in the constraint manager and padstack editor to understand which layer pairs exist in your design.

Understanding Allegro Drill File Output Structure

Allegro generates multiple files during NC drill output. Understanding each file’s purpose helps you provide correct data to manufacturers.

Files Generated by NC Drill Command

File	Extension	Contents	Needed by Manufacturer
Drill data	.drl, .tap	Hole coordinates and tool codes	Yes
Tool auto file	nc_tools_auto.txt	Tool size assignments	Sometimes
Drill statistics	.dts	Hole count summary	No
NC parameters	nc_param.txt	Export settings record	No

Send only the .drl or .tap files to manufacturing unless they specifically request tool table files. The metadata files serve as references for your own records.

Files Generated by NC Route Command

File	Extension	Contents	Needed by Manufacturer
Route data	.rou	Slot and milling paths	Yes (if slots exist)

If your design contains slots or milled cutouts, you must generate and provide both drill and route files.

Best Practices for Reliable Drill Output

Following consistent practices prevents problems and reduces manufacturing delays.

Before Starting Drill Generation

Run Manufacture → NC → Drill Customization to verify that all padstacks have proper drill definitions. Missing drill information in padstacks causes holes to not appear in output.

Check your constraint manager for via definitions that may span unexpected layer pairs.

During Configuration

Match every parameter between Gerber General Parameters and NC Parameters. Document your settings in a text file for future reference and troubleshooting.

Enable Enhanced Excellon Format and Auto Tool Select in every case unless your manufacturer explicitly requests otherwise.

After Generation

Verify files in an independent Gerber viewer before sending to manufacturing. Check alignment, scale, and hole count against your design.

Create a readme file documenting which drill file corresponds to which layer pair for multilayer designs with blind or buried vias.

Useful Resources for Allegro Users

Official Cadence Resources

Resource	Description
Cadence Online Support	Technical documentation and knowledge base
Cadence Community Forums	User discussions and expert responses
Allegro PCB Editor Help	Built-in documentation

Manufacturer-Specific Guides

Manufacturer	Documentation URL
OSH Park	docs.oshpark.com/design-tools/cadence-allegro
PCBWay	pcbway.com/blog/help_center
Seeed Fusion	seeedstudio.com/blog (Allegro export guide)
Sierra Circuits	protoexpress.com/blog

Gerber Viewer Downloads

Tool	Source
Gerbv	gerbv.github.io
ViewMate	pentalogix.com
GC-Prevue	graphicode.com

Frequently Asked Questions

Why does Allegro generate multiple drill files for my design?

Allegro creates separate drill files for each unique layer pair in your design. If you have through-holes spanning layers 1-4 and blind vias spanning layers 1-2, you get two drill files. The filename includes the layer numbers (designname-1-4.drl and designname-1-2.drl) to identify which file contains which holes. Additionally, if you enabled separate files for plated and non-plated holes, each layer pair generates two files, one for PTH and one for NPTH. This separation is actually preferred by manufacturers because different hole types require different processing steps.

What is the difference between NC Drill and NC Route in Allegro?

NC Drill generates coordinate data for circular holes only. This covers vias, component through-holes, and mounting holes. NC Route generates path data for non-circular features like slots, oblong holes, and board cutouts. If your design contains any slots or milled features, you must generate both NC Drill and NC Route files and provide both to your manufacturer. The NC Route command is accessed through Manufacture → NC → NC Route and produces .rou files.

Why does my manufacturer say the drill file format is wrong?

The most common cause is that Enhanced Excellon Format was not enabled in NC Parameters before generating drill files. Allegro’s default output uses a non-standard format that many manufacturer systems cannot interpret. Open NC Parameters (Manufacture → NC → NC Parameters), enable Enhanced Excellon Format and Auto Tool Select, then regenerate your drill files. Also verify that your units, format, and zero suppression settings match your Gerber artwork settings.

How do I match drill file settings to Gerber settings in Allegro?

Access both the Gerber settings (Manufacture → Artwork → General Parameters tab) and NC Parameters (Manufacture → NC → NC Parameters) and verify that identical values appear for: Output Units (inches or metric), Format (2.4 for inches, 3.3 for metric), Zero Suppression (Leading recommended), and Coordinate type (Absolute recommended). Mismatched settings between these two dialogs cause the most common drill alignment problems that manufacturers report.

Can I generate a single drill file for a design with blind and buried vias?

No, and you should not want to. Blind and buried vias require sequential lamination and drilling operations that occur at different stages of fabrication. Manufacturers need separate drill files for each layer pair so they can process each drilling operation at the correct point in the build sequence. Allegro automatically generates these separate files when you select Layer Pair output. Provide all generated drill files to your manufacturer along with documentation identifying which layers each file addresses. The filenames include layer numbers to assist with identification.

Working with NC Route for Slots and Cutouts

Allegro separates slot and milling data from circular drill holes. When your design contains oblong pads, slots, or internal cutouts, NC Drill alone will not capture this information.

When NC Route is Required

Feature	NC Drill	NC Route
Round holes	Yes	No
Oblong holes	No	Yes
Slots	No	Yes
Board cutouts	No	Yes
Internal routing	No	Yes

Access NC Route through Manufacture → NC → NC Route. Configure parameters similarly to NC Drill, ensuring units and format match your other manufacturing files.

The generated .rou file uses the same Excellon format commands but includes G01 (linear) and G02/G03 (arc) movements to define milling paths. Manufacturers need both .drl and .rou files when your design includes any routed features.

Conclusion

Generating NC drill files in Cadence Allegro requires attention to parameter configuration that other PCB design tools handle automatically. The critical steps involve enabling Enhanced Excellon Format and Auto Tool Select in NC Parameters, matching all settings with your Gerber artwork configuration, and understanding that separate files generate for different layer pairs and hole types.

Take time to verify drill files in an independent Gerber viewer before manufacturing submission. The few minutes spent on verification saves days of delay when manufacturers cannot process incorrectly formatted files.

With proper configuration, Allegro produces drill files that any manufacturer can use directly without questions or format interpretation problems.