How to Generate Gerber Files from Cadence Allegro

If you have ever tried to export Gerber files from Cadence Allegro or OrCAD PCB Editor, you know it is not exactly intuitive. Unlike KiCad or Eagle where a simple CAM processor gets the job done in minutes, Allegro takes a bottom-up approach that requires you to manually configure each “film” before exporting anything. I have seen entire engineering teams struggle with this process, and fabricators regularly receive incomplete packages from Allegro users who missed a step somewhere.

This guide cuts through the complexity and gives you a reliable, step-by-step method to generate Gerber files from Cadence Allegro that your PCB manufacturer will actually accept. Whether you are running Allegro 16.x, 17.x, or the latest OrCAD release, the fundamental workflow remains the same.

Understanding Gerber Files and Films in Cadence Allegro

Before diving into the export process, it helps to understand Allegro’s terminology. What most PCB software calls “layers,” Allegro refers to as “films,” a term that dates back to when photoplotters exposed actual photographic film for PCB manufacturing. Each film corresponds to a single Gerber file representing one layer of your board.

A complete manufacturing package from Cadence Allegro typically includes these essential files:

Film Type	Description	Required
Top Copper	Signal traces on component side	Yes
Bottom Copper	Signal traces on solder side	Yes
Top Solder Mask	Protective coating openings on top	Yes
Bottom Solder Mask	Protective coating openings on bottom	Yes
Top Silkscreen	Component labels on top	Optional
Bottom Silkscreen	Component labels on bottom	Optional
Board Outline	Physical board dimensions	Yes
Paste Top	Solder paste stencil for SMT	Assembly only
Paste Bottom	Solder paste stencil for SMT	Assembly only
NC Drill File	Hole locations and sizes	Yes

For multi-layer boards, you will also need inner copper layers and potentially inner plane layers. The solder mask and drill files are non-negotiable—without them, your fabricator cannot manufacture the board correctly, even if they have perfect copper artwork.

Pre-Export Checklist for Cadence Allegro

Running through these checks before generating Gerber files saves time and prevents embarrassing re-submissions to your manufacturer.

Run Status and Database Checks

Open your board file (.brd) in Allegro PCB Editor and verify the design status. Navigate to Tools → Database Check and ensure all results display green. Red or yellow warnings indicate problems that could translate into manufacturing defects or incomplete Gerber output.

Common issues flagged by database check include:

• Unconnected pins or dangling traces
• Overlapping geometry causing short circuits
• Missing padstack definitions
• Constraint violations

Address these issues before proceeding. A clean database check does not guarantee perfect Gerbers, but a failing check almost guarantees problems.

Verify Design Rule Check (DRC) Status

Run a final DRC by selecting Tools → Quick Reports → DRC. Clear any violations or document them explicitly in your fabrication notes. Pay particular attention to:

• Minimum trace width violations
• Clearance errors between copper features
• Drill-to-copper spacing issues
• Solder mask expansion problems

Confirm Layer Stackup

Double-check your layer stackup definition matches your intended board construction. Go to Setup → Cross-section and verify the layer order, materials, and thicknesses are correct. This information affects how Allegro generates artwork for inner layers, particularly for negative plane layers.

Setting Up Views in Cadence Allegro for Gerber Generation

Allegro uses Views to group related design elements that should appear together on a single film. You will create separate Views for each Gerber layer before exporting. This step is unique to Allegro and trips up many engineers accustomed to other PCB tools.

Accessing the Color Dialog

Press Ctrl+F5 or navigate to Setup → Colors to open the Color Dialog. This is where you configure which subclasses appear in each View.

Creating Views for Each Gerber Layer

In the Color Dialog, you will notice a Views dropdown that may be empty initially. For each Gerber file you need to generate, create a View containing only the relevant subclasses:

For Top Copper Film:

• ETCH/TOP
• PIN/TOP
• VIA CLASS/TOP
• BOARD GEOMETRY/OUTLINE (for reference)

For Bottom Copper Film:

• ETCH/BOTTOM
• PIN/BOTTOM
• VIA CLASS/BOTTOM

For Solder Mask Films:

• BOARD GEOMETRY/SOLDERMASK_TOP or SOLDERMASK_BOTTOM
• PIN subclasses as needed
• VIA CLASS as needed

Save each View configuration with a descriptive name that matches its purpose. This makes the film control setup much easier in the next step.

Generating Gerber Files Using the Artwork Control Form

With Views configured, you are ready to export Gerber files. Navigate to Manufacture → Artwork to open the Artwork Control Form. This dialog contains two critical tabs: General Parameters and Film Control.

Configuring General Parameters in Allegro

Click the General Parameters tab and configure these essential settings:

Parameter	Recommended Setting	Notes
Device Type	Gerber RS274X	Industry standard format
Output Units	Inches or Millimeters	Match your design units
Format	2.4 (Imperial) or 3.3 (Metric)	Precision settings
Film Size Limits	14 x 16 or larger	Must exceed board size
Undefined Line Width	0.1mm or 4 mils	Prevents zero-width errors

The Undefined Line Width setting deserves special attention. Allegro defaults this to zero, which causes problems when your board outline or other geometry has no explicit line width assigned. Set this to at least 0.1mm (approximately 4 mils) to ensure all lines appear in your Gerber output. Zero-width lines are invisible to your fabricator and can result in missing board outlines.

Adding Films to the Artwork Control Form

Switch to the Film Control tab. Here you will add individual films for each Gerber layer. The process works as follows:

Step 1: Right-click on an existing folder (like TOP) and select Add Manual

Step 2: Enter a descriptive film name such as OUTLINE, TOP_COPPER, or SOLDERMASK_TOP

Step 3: In the Subclass Selection window, expand the relevant categories and check the appropriate subclasses

Step 4: Click OK to add the film to your Available Films list

Repeat this process for each required layer. For a standard two-layer board, you need at minimum:

• OUTLINE (Board Geometry → DESIGN_OUTLINE or OUTLINE)
• TOP_COPPER (ETCH/TOP, PIN/TOP, VIA CLASS/TOP)
• BOTTOM_COPPER (ETCH/BOTTOM, PIN/BOTTOM, VIA CLASS/BOTTOM)
• SOLDERMASK_TOP (appropriate mask subclasses)
• SOLDERMASK_BOTTOM (appropriate mask subclasses)
• SILKSCREEN_TOP (SILKSCREEN_TOP subclass)
• SILKSCREEN_BOTTOM (SILKSCREEN_BOTTOM subclass)

Creating the Gerber Artwork Files

Once all films are configured:

1. Click Select All at the bottom of the Available Films list
2. Click Create Artwork
3. Monitor the log window for errors or warnings
4. Click OK when complete

Allegro generates the Gerber files in a subdirectory called “artwork” within your project folder. Files typically receive .art extensions, though some versions use .pho extensions.

Generating NC Drill Files from Cadence Allegro

Gerber files alone cannot manufacture your PCB. You need NC drill files that specify hole locations and sizes. This is a separate export process in Allegro and is frequently overlooked by new users.

Accessing the NC Drill Dialog

Navigate to Manufacture → NC → NC Drill to open the NC Drill configuration window.

Configuring NC Drill Parameters

Before generating the drill file, click Parameters (or NC Parameters in some versions) to access critical settings:

Parameter	Recommended Setting	Why It Matters
Enhanced Excellon Format	Enabled	Modern drill format
Leading Zero Suppression	Enabled	Standard convention
Output Units	Match Gerber settings	Prevents alignment issues
Coordinates	Absolute	Most compatible option

Critical Setting: Enable Enhanced Excellon Format. By default, Allegro does not export in Excellon format, which causes compatibility problems with many fabricators and Gerber viewers. This single checkbox solves most drill file issues.

Generating the Drill File

Back in the NC Drill window:

1. Verify the output file name and location
2. Check Auto Tool Select to automatically assign drill tool numbers
3. Check Repeat codes for optimized output
4. Click Drill to generate the file

The drill file appears in your project directory with a .drl or .tap extension. Some Allegro versions also generate supporting files like nc_param.txt containing drill metadata.

Creating Drill Legends (Optional)

For comprehensive documentation, generate a drill legend showing hole sizes and symbols. Navigate to Manufacture → NC → Drill Legend and configure the parameters. This creates a visual reference chart that helps fabricators verify drill tool assignments.

Cadence Allegro Gerber File Extensions and Naming Conventions

Allegro uses file extensions that differ from the Protel/Altium conventions most fabricators expect. Understanding these extensions helps you verify your export and communicate with manufacturers.

Allegro Extension	Layer Type	Equivalent Protel Extension
.art	Artwork (any layer)	Various
.pho	Photo plot output	Various
TOP.art	Top copper	.GTL
BOT.art	Bottom copper	.GBL
SMT.art	Solder mask top	.GTS
SMB.art	Solder mask bottom	.GBS
SST.art	Silkscreen top	.GTO
SSB.art	Silkscreen bottom	.GBO
.drl	Drill file	.TXT or .DRL
.tap	Drill file (TAP format)	.TXT

Many fabricators can handle Allegro naming conventions, but if you encounter issues, consider renaming files to match standard Protel extensions. The actual file content remains valid regardless of the extension.

Common Gerber Generation Problems in Cadence Allegro

Missing Board Outline in Gerber Files

This problem affects Allegro users constantly. The board outline must exist on a proper subclass (typically BOARD GEOMETRY/OUTLINE or BOARD GEOMETRY/DESIGN_OUTLINE) and must be explicitly included in your artwork film definition.

Solution: Create a dedicated OUTLINE film that includes only the BOARD GEOMETRY/OUTLINE subclass. Verify the outline is a closed polygon with non-zero line width.

Zero-Width Lines Not Appearing

If your board outline or other geometry has zero line width assigned, it will not appear in the Gerber output.

Solution: In General Parameters, set Undefined Line Width to at least 0.1mm or 4 mils.

Drill Holes Misaligned with Pads

Drill misalignment typically results from mismatched units or coordinate origins between Gerber and drill exports.

Solution: Ensure Output Units and Coordinate settings match exactly between Artwork Control Form and NC Drill parameters. Use absolute coordinates for both.

Drill File Not in Excellon Format

Some Gerber viewers and fabricators cannot read Allegro’s default drill format.

Solution: Enable Enhanced Excellon Format in NC Drill Parameters before generating the drill file.

Missing Solder Mask Layers

Users frequently export copper and outline but forget solder mask layers, which are essential for proper board coating.

Solution: Always create separate films for SOLDERMASK_TOP and SOLDERMASK_BOTTOM. Verify both appear in your final file package.

Verifying Your Cadence Allegro Gerber Output

Before sending files to manufacturing, verify them in an independent viewer. Do not rely solely on Allegro’s built-in viewing.

Recommended verification steps:

1. Load all Gerber files into a third-party viewer
2. Overlay the drill file on copper layers to check alignment
3. Verify board outline dimensions match your design intent
4. Confirm solder mask openings align with pads
5. Check silkscreen does not overlap solder mask openings

Package all required files into a single .zip archive. Include only manufacturing files, not temporary files or project databases.

Useful Resources for Cadence Allegro Gerber Generation

Official Cadence Resources:

• Cadence PCB Training Videos: https://resources.pcb.cadence.com/trainingvideos
• Allegro PCB Editor Documentation: https://www.cadence.com/en_US/home/tools/pcb-design-and-analysis/pcb-layout/allegro-pcb-designer.html

Gerber Viewers:

• Gerbv (Open Source): http://gerbv.geda-project.org/
• ViewMate (Free): https://www.pentalogix.com/viewmate
• HQDFM (Free DFM Analysis): https://dfm.hqpcb.com/

Fabricator Guidelines:

• OSH Park Allegro Guide: https://docs.oshpark.com/design-tools/cadence-allegro/
• PCBWay Allegro Tutorial: https://www.pcbway.com/blog/help_center/How_to_Generate_Gerber_in_Cadence_Allegro_d66fff3a.html
• Seeed Fusion Allegro Guide: https://www.seeedstudio.com/blog/2019/12/13/how-to-generate-pcb-gerber-files-from-cadence-allegro-orcad/

Gerber Format Specification:

• UCAMCO Gerber Format: https://www.ucamco.com/en/gerber

Frequently Asked Questions

What is the difference between Allegro and OrCAD for Gerber generation?

Allegro and OrCAD PCB Editor share the same interface and Gerber export process. The main difference is licensing—Allegro targets advanced high-speed designs while OrCAD handles mid-range complexity at a lower price point. The Artwork Control Form and NC Drill procedures are identical in both products.

Why do my Gerber files have .art extensions instead of standard extensions?

Allegro uses .art (artwork) extensions by default. Most modern fabricators can process these files regardless of extension. If your manufacturer requires standard extensions (.GTL, .GBL, etc.), you can safely rename the files. The content format remains Gerber RS274X, which is universally compatible.

How do I export Gerber files for a multi-layer board in Allegro?

For multi-layer boards, create additional films for each inner layer in the Artwork Control Form. Inner signal layers use subclasses like ETCH/IN1, ETCH/IN2, etc. Inner planes may require negative polarity settings depending on your stackup. Also ensure your NC Drill export includes all drill pairs for blind and buried vias if applicable.

Why does my fabricator say the drill file is not in the correct format?

Allegro’s default drill output is not Excellon format, which causes compatibility issues. Go to Manufacture → NC → NC Drill, click Parameters, and enable Enhanced Excellon Format. Regenerate the drill file and resubmit to your fabricator.

Can I automate Gerber generation in Cadence Allegro?

Yes, Allegro supports SKILL programming for automation. You can create scripts that configure artwork films, set parameters, and generate outputs automatically. For simpler needs, save your Artwork Control Form configuration with all films defined, then reuse it across projects by clicking Select All and Create Artwork after verifying layer assignments.

Final Recommendations for Allegro Gerber Export

Generating Gerber files from Cadence Allegro requires more manual configuration than most modern PCB tools, but the process becomes routine once you understand the workflow. Create a standard set of film definitions that you reuse across projects. Document your General Parameters settings and NC Drill configuration so you can replicate successful exports.

Always verify your output in an independent Gerber viewer before sending to manufacturing. The few minutes spent checking alignment and completeness prevents costly delays and board re-spins. Keep your fabricator’s specific requirements on hand, as some manufacturers have preferences for file naming, format settings, or additional documentation.

With practice, Allegro’s Gerber generation becomes second nature, and the software’s detailed control over each film actually provides flexibility that simpler tools lack.