Understanding Gerber File Extensions and Layer Naming: Complete PCB Engineer’s Guide

The first time I submitted Gerber files to a manufacturer and got an email asking “which file is your top copper layer?”, I realized that understanding Gerber file extensions isn’t optional—it’s essential. Every PCB design tool uses different naming conventions, and what seems obvious to you might be completely cryptic to your fab house. This guide breaks down the logic behind Gerber file extensions and layer naming so you can communicate clearly with any manufacturer, anywhere in the world.

What Are Gerber File Extensions?

Gerber file extensions are the suffix characters after the filename that identify which PCB layer each file represents. Unlike most file formats where the extension indicates the file type (like .pdf or .docx), Gerber extensions serve a dual purpose: they confirm the file is a Gerber format AND specify the layer function.

The official standard extension for Gerber files is simply .GBR or .gbr. However, the PCB industry has developed informal conventions where the extension itself communicates layer information. These conventions evolved from Protel (now Altium Designer) and have become widely recognized across the industry.

Why Layer Naming Matters for Manufacturing

Impact	Consequence of Poor Naming
Layer identification	Manufacturer guesses layer function
Stackup order	Inner layers assembled incorrectly
Production delays	Back-and-forth clarification emails
Board failures	Wrong layer used in wrong position
Cost increases	Engineering time to interpret files

When manufacturers receive your Gerber package, their CAM software attempts to automatically identify each layer based on the file extension. Clear naming means automatic recognition. Unclear naming means manual interpretation—which introduces delay and error potential.

The Protel/Altium Naming Convention

The Protel naming convention has become the de facto industry standard for Gerber file extensions. Most manufacturers worldwide recognize these extensions instantly, and most automated import systems are designed around them.

Protel Extension Logic

The naming follows a simple pattern: G + Position + Layer Type

• G = Gerber
• T = Top, B = Bottom
• Layer Type = L (Layer/copper), S (Solder mask), O (Overlay/silkscreen), P (Paste)

Complete Protel Extension Reference

Extension	Layer Name	Description
.GTL	Top Copper	Top signal layer with traces, pads, copper pours
.GBL	Bottom Copper	Bottom signal layer
.GTS	Top Solder Mask	Defines solder mask openings on top
.GBS	Bottom Solder Mask	Defines solder mask openings on bottom
.GTO	Top Silkscreen	Component labels, logos on top (overlay)
.GBO	Bottom Silkscreen	Component labels on bottom
.GTP	Top Paste	Stencil openings for top-side SMT
.GBP	Bottom Paste	Stencil openings for bottom-side SMT
.GKO	Keep-Out/Outline	Board boundary definition
.GM1	Mechanical 1	Often used for board outline
.G1, .G2	Inner Layer 1, 2	Inner signal layers
.GP1, .GP2	Inner Plane 1, 2	Power/ground plane layers

This convention works because it’s both human-readable and machine-parseable. A CAM engineer in any country can look at “.GTS” and immediately know it’s the top solder mask, regardless of what language they speak.

Gerber File Extensions by CAD Software

Every PCB design tool has its own default naming convention. Understanding these differences helps you work with files from colleagues using different software and explains why manufacturers sometimes request file renaming.

Altium Designer Extensions

Altium follows the Protel convention directly, which makes sense given Altium acquired Protel.

Layer	Altium Extension
Top Copper	.GTL
Bottom Copper	.GBL
Top Solder Mask	.GTS
Bottom Solder Mask	.GBS
Top Silkscreen	.GTO
Bottom Silkscreen	.GBO
Top Paste	.GTP
Bottom Paste	.GBP
Board Outline	.GKO or .GM1
Inner Signal	.G1, .G2, .G3…
Inner Plane	.GP1, .GP2…
Drill File	.DRL or .TXT

KiCad Default Extensions

KiCad uses descriptive layer names rather than coded extensions by default. This approach is more readable but may not be automatically recognized by all manufacturer systems.

Layer	KiCad Default	With Protel Option
Top Copper	F_Cu.gbr	.GTL
Bottom Copper	B_Cu.gbr	.GBL
Top Solder Mask	F_Mask.gbr	.GTS
Bottom Solder Mask	B_Mask.gbr	.GBS
Top Silkscreen	F_Silkscreen.gbr	.GTO
Bottom Silkscreen	B_Silkscreen.gbr	.GBO
Top Paste	F_Paste.gbr	.GTP
Bottom Paste	B_Paste.gbr	.GBP
Board Outline	Edge_Cuts.gbr	.GKO
Drill (PTH)	PTH.drl	.DRL
Drill (NPTH)	NPTH.drl	.DRL

Recommendation: Enable “Use Protel filename extensions” in KiCad’s plot settings for maximum manufacturer compatibility. This single checkbox eliminates most naming-related issues.

Eagle (Autodesk) Extensions

Eagle uses a different convention that predates the Protel standard. Some extensions are intuitive, others require translation.

Layer	Eagle Extension	Equivalent Protel
Top Copper	.cmp or .top	.GTL
Bottom Copper	.sol or .bot	.GBL
Top Solder Mask	.stc or .tsm	.GTS
Bottom Solder Mask	.sts or .bsm	.GBS
Top Silkscreen	.plc or .tsk	.GTO
Bottom Silkscreen	.pls or .bsk	.GBO
Top Paste	.crc or .tsp	.GTP
Bottom Paste	.crs or .bsp	.GBP
Board Outline	.dim or .gml	.GKO
Drill File	.drl or .xln	.DRL

Many manufacturers provide Eagle-specific CAM job files that output Protel-compatible extensions. Using these pre-configured jobs simplifies the export process considerably.

OrCAD/Allegro Extensions

OrCAD typically outputs files with .art or .PHO extensions, which don’t indicate layer function at all.

Layer	OrCAD Default	Notes
Top Copper	TOP.art or .PHO	Requires renaming
Bottom Copper	BOT.art	Requires renaming
Top Solder Mask	SMT.art	Requires renaming
Bottom Solder Mask	SMB.art	Requires renaming
Top Silkscreen	SST.art	Requires renaming
Bottom Silkscreen	SSB.art	Requires renaming
Drill File	.tap or .drl	Check format settings

Important: Many manufacturers request that OrCAD users rename files to Protel conventions before submission because .art and .PHO extensions aren’t automatically recognized by standard CAM systems.

PADS Extensions

PADS uses .PHO (photoplot) extensions with layer information encoded in the filename rather than the extension.

Layer	PADS Format
Top Copper	filename_top.PHO
Bottom Copper	filename_bot.PHO
Solder Mask	filename_sm*.PHO
Silkscreen	filename_ss*.PHO

The .PHO extension refers to the original photoplotter output format. While functional, this convention may cause confusion with automated systems expecting Protel extensions.

Understanding PCB Layer Types

Beyond extensions, understanding what each layer represents helps you verify your Gerber output is complete and correct.

Copper Layers

Copper layers contain all conductive features: signal traces, component pads, via pads, and copper pours. For a standard two-layer board, you need top copper (.GTL) and bottom copper (.GBL). Multilayer boards add inner layers (.G1, .G2, etc.) and potentially plane layers (.GP1, .GP2).

Viewing orientation: All Gerber layers are viewed as if looking through the board from the top. This means bottom layers appear mirrored—traces that run left-to-right on the physical bottom surface appear right-to-left in the Gerber viewer. This is correct and expected.

Solder Mask Layers

Solder mask files define where the protective coating (typically green) will NOT be applied. These layers use negative polarity—drawn features represent openings in the mask that expose copper for soldering.

Solder Mask Consideration	Details
Polarity	Negative (drawn = opening)
Expansion	Typically 2-4 mil larger than pads
Via treatment	Covered (tented) or exposed
File count	Two files: top (.GTS) and bottom (.GBS)

Silkscreen Layers

Silkscreen (also called overlay or legend) layers contain printed markings: component designators (R1, C5, U3), polarity indicators, logos, and assembly notes. These layers are optional but highly recommended for assembly reference.

Common silkscreen issues:

• Text overlapping pads (prevents soldering)
• Text extending beyond board outline
• Text too small to print legibly (minimum 0.8mm height)

Paste Mask Layers

Paste layers define stencil openings for solder paste application during SMT assembly. These files are only needed if your board includes surface mount components and you’re ordering assembly services or a separate stencil.

Board Outline Layer

The outline (also called mechanical or keep-out) layer defines the physical boundary of your PCB. Without this layer, manufacturers cannot determine where to cut individual boards from the production panel.

Outline Extension	Source
.GKO	Protel/Altium
.GM1	Altium Mechanical 1
Edge_Cuts.gbr	KiCad
.dim	Eagle
.FAB	OrCAD

Critical: The outline must be a closed shape with no gaps. Open outlines cause manufacturing holds while engineers request clarification.

Drill Files

Drill files aren’t technically Gerber format—they use Excellon or NC drill format—but they’re always submitted alongside Gerber files and follow similar naming patterns.

Drill Extension	Format
.DRL	Common Excellon
.XLN	Excellon
.TXT	ASCII drill (Altium)
.NC	Numerical control
.TAP	Older format

Drill files should be clearly separated into plated (PTH) and non-plated (NPTH) holes when your design includes both types.

Layer Naming Best Practices

Following consistent naming practices prevents confusion and manufacturing delays regardless of which CAD tool you use.

Use Recognized Conventions

The safest approach is using Protel extensions because they’re universally recognized. If your CAD tool doesn’t output these by default, either configure it to do so or rename files before submission.

Include a Layer Mapping Document

When file names might be ambiguous, include a simple text or PDF file that maps each filename to its layer function:

LAYER MAPPING – Project XYZ Rev 2.1===================================project_xyz.GTL – Top Copperproject_xyz.GBL – Bottom Copper  project_xyz.GTS – Top Solder Maskproject_xyz.GBS – Bottom Solder Maskproject_xyz.GTO – Top Silkscreenproject_xyz.GKO – Board Outlineproject_xyz.DRL – Drill File (PTH)

This takes two minutes to create and can save days of back-and-forth communication.

Maintain Consistency

Don’t mix naming conventions within the same project. If you use Protel extensions for copper layers, use them for all layers. Mixed conventions confuse both automated systems and human reviewers.

Include Version Information

Consider including revision numbers or dates in your Gerber folder name (not individual file names):

• Good: ProjectName_Rev2.1_Gerbers/
• Avoid: project_rev2_GTL.GTL (redundant, confusing)

Gerber X2 FileFunction Attribute

Modern Gerber X2 format includes a standardized method for identifying layer function that doesn’t rely on file extensions at all.

How FileFunction Works

X2 files embed metadata directly within the Gerber file that explicitly declares the layer’s purpose:

%TF.FileFunction,Copper,L1,Top*%%TF.FileFunction,Soldermask,Top*%%TF.FileFunction,Legend,Top*%

This eliminates ambiguity because the layer function is machine-readable and standardized, regardless of what filename or extension you use.

FileFunction Layer Declarations

FileFunction Value	Layer Purpose
Copper,L1,Top	Top copper layer
Copper,L2,Bot	Bottom copper layer
Copper,L2,Inr	Inner copper layer
Soldermask,Top	Top solder mask
Soldermask,Bot	Bottom solder mask
Legend,Top	Top silkscreen
Legend,Bot	Bottom silkscreen
Paste,Top	Top paste/stencil
Paste,Bot	Bottom paste/stencil
Profile,NP	Board outline (non-plated)

X2 Adoption Status

While X2 is the official current standard, not all manufacturers and CAM systems fully support it yet. The safest approach is using both X2 attributes (if your CAD tool supports them) AND clear file extensions. This provides redundancy—modern systems read the attributes while older systems fall back to extension-based identification.

Useful Resources for Gerber File Management

Gerber Viewers (Free)

Tool	Platform	URL
Gerbv	Windows, Linux, Mac	gerbv.github.io
KiCad GerbView	Windows, Linux, Mac	kicad.org
ViewMate	Windows	pentalogix.com
HQDFM Online	Browser	nextpcb.com/free-online-gerber-viewer
Reference Gerber Viewer	Browser	gerber-viewer.ucamco.com

Manufacturer CAM Job Files

Manufacturer	CAD Support	URL
JLCPCB	Eagle, KiCad	jlcpcb.com/help
PCBWay	Multiple	pcbway.com/helpcenter
OSH Park	KiCad, Eagle	docs.oshpark.com
Seeed Studio	Eagle	seeedstudio.com

Official Documentation

Resource	Description	URL
Ucamco Gerber Spec	Official format specification	ucamco.com/gerber
Gerber Layer Format	Technical documentation	ucamco.com/en/guest/downloads
IPC Standards	Industry PCB standards	ipc.org

Frequently Asked Questions

What is the official standard Gerber file extension?

The official standard extension is .GBR or .gbr according to Ucamco, who maintains the Gerber format specification. However, industry practice commonly uses layer-specific extensions like .GTL, .GBL, .GTS based on the Protel/Altium convention. While using .GBR for everything is technically correct, it requires the filename itself to clearly indicate layer function, and many automated CAM systems won’t automatically recognize layer assignments. For maximum compatibility with manufacturers worldwide, the Protel convention remains the practical choice.

Why does my manufacturer request Protel extensions when I use KiCad?

Manufacturer CAM systems are typically configured to automatically detect and assign layers based on Protel extensions. KiCad’s default descriptive names (F_Cu.gbr, B_Mask.gbr) are human-readable but may not trigger automatic layer recognition in older or differently-configured CAM software. Enabling “Use Protel filename extensions” in KiCad’s plot dialog generates extensions that these systems recognize automatically, reducing the chance of layer misidentification and eliminating the need for manual file renaming or mapping.

How do I handle inner layer naming for multilayer boards?

Inner signal layers use sequential numbering: .G1, .G2, .G3, etc., counting from top to bottom after the top copper layer. Inner plane (power/ground) layers use .GP1, .GP2, etc. For complex stackups, always include a stackup document that clearly shows the layer order, material types, and copper weights. This is especially important because inner layer sequence cannot be visually verified from Gerber files alone—the manufacturer needs explicit documentation to build your board correctly.

Should I use Gerber X2 attributes or stick with traditional extensions?

Use both when possible. Gerber X2 FileFunction attributes provide machine-readable layer identification that eliminates ambiguity, but not all manufacturers fully support X2 yet. By using X2-enabled export AND clear Protel-style extensions, you get the benefits of modern metadata for X2-capable systems while maintaining backward compatibility with traditional CAM workflows. If you must choose one, Protel extensions currently offer broader manufacturer compatibility.

What happens if I submit Gerber files with unclear or wrong extensions?

At best, your manufacturer’s CAM engineer will contact you for clarification, adding 1-2 days to your timeline. At worst, layers may be misidentified and your board produced incorrectly—top silkscreen swapped with bottom, inner layers in wrong sequence, or solder mask applied where copper should be exposed. These errors often aren’t caught until boards arrive and don’t work. The few minutes spent on proper naming prevents expensive mistakes and respins.

Conclusion

Gerber file extensions and layer naming might seem like minor details compared to circuit design and layout work, but they’re the critical link between your design intent and what actually gets manufactured. The Protel naming convention (.GTL, .GBL, .GTS, etc.) has become the industry standard for good reason—it’s logical, widely recognized, and works with virtually every manufacturer’s CAM system.

Whether you use Altium, KiCad, Eagle, or OrCAD, take the time to configure your Gerber output for clear, standard naming. Enable Protel extensions where available, include a layer mapping document for complex boards, and verify your files in a Gerber viewer before submission. These simple practices eliminate an entire category of manufacturing problems and ensure your carefully designed boards are built exactly as intended.

The few minutes spent on proper file organization pays back many times over in faster quotes, smoother production, and boards that work the first time.