Common Gerber File Errors and How to Fix Them: Complete Troubleshooting Guide

After fifteen years of submitting PCB designs for manufacturing, I’ve learned that Gerber file errors are simultaneously the most frustrating and most preventable problems in the production process. That email from your fab house asking for corrections always seems to arrive when you’re already behind schedule. The good news is that nearly every common Gerber file error follows predictable patterns, and knowing what to look for means you can catch these problems before they delay your boards. This guide covers the errors manufacturers see most frequently and provides practical solutions for each.

Why Gerber File Errors Happen

Gerber files translate your PCB design into manufacturing instructions. This translation process involves multiple software settings, file format choices, and layer configurations—each representing an opportunity for something to go wrong. Unlike schematic errors that trigger DRC warnings, many Gerber export problems slip through unnoticed until a manufacturer tries to import your files.

Impact of Gerber Errors on Production

Error Type	Production Impact	Typical Delay
Missing files	Cannot proceed, order held	1-3 days
Wrong format	Import failure, manual conversion	1-2 days
Layer misalignment	Potential board failure, scrap	Complete respin
Drill errors	Holes in wrong locations	Complete respin
Incomplete outline	Manual interpretation required	1-2 days
Empty/corrupted files	Cannot determine intent	1-3 days

Understanding what can go wrong helps you implement verification steps that catch problems before submission.

Missing or Incomplete Gerber Files

The most common Gerber file error is simply not including all the necessary files in your submission. Every layer of your PCB requires its own Gerber file, and missing even one can halt production.

Required Files for Standard Two-Layer Boards

Layer	Purpose	Common Extensions
Top Copper	Signal traces, pads	.GTL, .top, .cmp
Bottom Copper	Signal traces, pads	.GBL, .bot, .sol
Top Solder Mask	Pad exposure openings	.GTS, .stc
Bottom Solder Mask	Pad exposure openings	.GBS, .sts
Top Silkscreen	Component labels	.GTO, .sst, .plc
Bottom Silkscreen	Component labels	.GBO, .ssb, .pls
Board Outline	Physical boundary	.GKO, .gm1, .outline
Drill File	Hole locations and sizes	.DRL, .XLN, .drd

How to fix: Create a checklist for your specific layer count and verify every file exists before zipping. Open each file in a Gerber viewer to confirm it contains actual data—zero-byte files that appear in your folder won’t help the manufacturer.

Multilayer Board Additional Requirements

For boards with four or more layers, you need inner layer copper files plus potentially multiple drill files if using blind or buried vias.

Layer Count	Additional Files Required
4-layer	Inner layer 1, Inner layer 2
6-layer	Inner layers 1-4
8+ layers	All inner layers, stackup documentation
HDI boards	Multiple drill files per drill span

How to fix: Include a stackup document (PDF, Excel, or text file) that clearly identifies the order and purpose of each layer file. Without this information, manufacturers must guess at layer sequence.

Missing Board Outline

The board outline defines the physical boundary where your PCB will be routed from the panel. Without a clearly defined outline, manufacturers cannot determine where to cut your board.

Signs of Board Outline Problems

Problem	Symptom	Result
Missing outline file	No .GKO or similar in package	Production hold
Outline on wrong layer	Appears on silkscreen	Incorrect dimensions
Open outline	Gaps in boundary	Ambiguous board shape
Multiple outlines	Conflicting boundaries	Confusion over intent

How to fix in KiCad: Ensure all boundary geometry is on the Edge.Cuts layer. The outline must be a single closed shape—verify there are no gaps where line segments fail to meet.

How to fix in Eagle: Include both Layer 20 (Dimension) and Layer 46 (Milling) in your outline output. Internal cutouts often appear on the Milling layer and will be missed if you only export Dimension.

How to fix in Altium: Export the mechanical layer containing your board outline. Verify the Keep-Out layer matches your intended board boundary.

Missing or Incorrect Drill Files

Drill file problems rank among the most critical Gerber errors because they directly affect whether components can be mounted. A missing drill file means no holes—no vias, no through-hole components, no mounting holes.

Common Drill File Errors

Error	Cause	Consequence
Missing drill file	Separate export step forgotten	No holes drilled
Drill map instead of drill file	Wrong export option	Supplementary info only, not machinable
Wrong coordinate format	Settings mismatch	Holes in wrong locations
Wrong units	Inch vs. metric confusion	25.4x scaling error
Missing tool definitions	Incomplete header	Unknown hole sizes

Identifying the difference: A drill file (.DRL, .XLN) contains machine-readable NC code with coordinate data. A drill map is a visual reference document that cannot be used for manufacturing. If your file opens as an image rather than coordinate data, you exported the wrong thing.

How to fix coordinate format issues: Drill file headers should clearly specify the format. Look for lines indicating:

• Leading or trailing zero suppression
• Coordinate format (e.g., 2:4, 2:5, 3:3)
• Units (INCH or METRIC)

If your header is incomplete or your CAD tool doesn’t include this information, specify it in a readme file. Most manufacturers assume 2:4 format with trailing zero suppression when not specified.

Drill-to-Copper Misalignment

One of the most frustrating problems occurs when drill holes don’t align with copper pads. This typically results from different origin settings between Gerber and drill export.

Symptoms:

• Holes systematically offset from pad centers
• Scaling appears correct but position is wrong
• Problem affects all holes equally

How to fix:

1. Use the same coordinate origin for both Gerber and drill file export
2. In KiCad, enable “Use drill/place file origin” for both exports
3. In Eagle, verify your CAM job uses consistent origin settings
4. Open both files in a Gerber viewer and overlay them to verify alignment before submission

Obsolete or Wrong File Format

The industry standard format is RS-274X (Extended Gerber). Submitting files in older formats or manufacturer-specific formats causes import failures and delays.

Gerber Format Comparison

Format	Status	Compatibility
RS-274D (Standard Gerber)	Obsolete	Avoid—requires external aperture list
RS-274X (Extended Gerber)	Current standard	Universal acceptance
Gerber X2	Current	Wide but not universal support
Gerber X3	Draft	Limited support
ODB++	Alternative	Many manufacturers accept

How to fix format issues:

• Configure your CAD software to export RS-274X format
• If your manufacturer rejects X2 files, disable extended attributes and re-export
• Never submit native CAD files (.brd, .pcb, .kicad_pcb) unless specifically instructed—convert to Gerber first

Aperture List Problems

RS-274D files require a separate aperture list defining tool shapes and sizes. This external dependency creates opportunities for errors. RS-274X embeds aperture definitions within the file, eliminating this problem.

How to fix: If you must use RS-274D (you shouldn’t), ensure the aperture list format matches the Gerber file format and is included in your submission. Better solution: switch to RS-274X export.

Layer Misalignment Errors

When different layers of your PCB don’t align correctly in the Gerber files, the manufactured board won’t work. Traces might not connect to pads, solder mask might cover connections, and drill holes might miss their targets.

Causes of Layer Misalignment

Cause	Detection Method	Prevention
Different export origins	Overlay in viewer	Use consistent origin
Incremental vs. absolute coordinates	Check file headers	Force absolute mode
Different unit settings	Scaling appears wrong	Standardize on mm or inches
CAD software bugs	Appears after export	Update software, verify output

How to fix: Load all Gerber layers plus drill files into a viewer and overlay them. Toggle layers on and off to verify:

• Copper pads align with drill holes
• Solder mask openings expose the correct pads
• Silkscreen doesn’t overlap pads
• All layers share the same origin point

Consider adding fiducial marks to your design—these provide clear alignment references visible on multiple layers.

Solder Mask Errors

Solder mask problems affect solderability and board reliability. Common issues include missing openings over pads, excessive clearance, and incorrect polarity.

Common Solder Mask Problems

Problem	Visual Symptom	Manufacturing Result
Missing openings	Mask covers pads	Cannot solder components
Excessive clearance	Openings too large	Exposed copper between pads
Wrong polarity	File appears inverted	All copper exposed or covered
Empty mask file	No data exported	Manufacturer guesses intent

How to fix polarity issues: Solder mask Gerber files should be “positive”—the drawn areas represent where mask will be removed to expose copper. If your viewer shows solid mask covering everything or nothing, check your CAD export polarity setting.

Eagle 9.20+ specific fix: The CAM Processor defaults “Negative Polarity” checked for solder mask. Uncheck this option before processing.

How to fix empty solder mask files: Some CAD tools generate empty or malformed solder mask files when a layer has no exposed copper (vias only, tented). Verify your solder mask files contain valid Gerber commands, not just header information.

Silkscreen Problems

Silkscreen errors don’t prevent boards from functioning but create assembly problems and look unprofessional.

Silkscreen Issues and Fixes

Issue	Problem	Fix
Text on pads	Ink prevents soldering	Enable “subtract soldermask from silkscreen”
Missing designators	Components unidentified	Plot reference designators layer
Text too small	Illegible after printing	Minimum 0.8mm (32 mil) height
Bottom silkscreen missing	Only top exported	Manually add bottom silk output
Silkscreen extends past board	Prints on panel	Clip silkscreen to board outline

How to fix silkscreen on pads: Modern CAD tools include an option to automatically remove silkscreen from solder mask openings. In KiCad, enable “Subtract soldermask from silkscreen.” In Altium, this is handled by clearance rules.

Vectorized Pad Errors

Some CAD software exports surface mount pads as clusters of small vectors rather than single solid shapes. This phenomenon most commonly affects solder mask and paste mask layers.

Why it matters: Vectorized pads slow down CAM processing, may cause imaging problems during fabrication, and increase file sizes unnecessarily.

How to fix: Configure your CAD software to generate “flash pads” instead of “vector pads.” The exact setting location varies by tool:

• In Altium, check the Gerber export options for pad generation method
• In older Eagle versions, this may require CAM job modification
• If stuck with vectorized files, ask your manufacturer if they can process them (most can, with extra time)

Composite Layer Errors

When CAD software splits a single copper layer into multiple Gerber files (one for pours, one for traces, one for pads), manufacturers must manually reconstruct the complete layer.

How to fix: Check your CAD export settings to ensure each physical layer exports as a single Gerber file. In some tools, this requires disabling “separate positive and negative” or similar options. Verify by loading your exported files—you should have exactly one file per physical layer.

Unclear File Naming

While not technically an error, unclear file names increase the risk of manufacturers misinterpreting your design.

File Naming Best Practices

Do	Don’t
Use Protel extensions (.GTL, .GBL)	Use generic extensions (.gbr for all)
Include layer description	Use numbers only (layer1.gbr)
Match your stackup document	Use your CAD tool’s cryptic defaults
Be consistent across projects	Change conventions randomly

How to fix: Enable “Protel filename extensions” in KiCad. In Eagle, use manufacturer-provided CAM jobs that include proper naming. Create or download a naming convention reference and follow it consistently.

How to Verify Your Gerber Files Before Submission

Prevention is easier than fixing problems after submission. Implement these verification steps before every order.

Pre-Submission Verification Checklist

Step	What to Check	Tool
1. File completeness	All layers present	File manager
2. File validity	No zero-byte files	Gerber viewer
3. Layer alignment	All layers register	Gerber viewer overlay
4. Drill alignment	Holes centered on pads	Gerber viewer overlay
5. Solder mask	Pads exposed correctly	Gerber viewer
6. Outline	Closed, no gaps	Gerber viewer
7. DFM check	Manufacturing violations	Online DFM tool

Useful Resources for Verification

Tool	Type	URL
HQDFM (NextPCB)	Online viewer + DFM	nextpcb.com/free-online-gerber-viewer
Gerbv	Free desktop viewer	gerbv.github.io
ViewMate	Free/paid desktop viewer	pentalogix.com
KiCad GerbView	Free desktop viewer	kicad.org
Altium 365 Viewer	Online viewer	altium.com/viewer
JLCPCB Viewer	Online viewer + order	jlcpcb.com
PCBWay Viewer	Online viewer + order	pcbway.com

Frequently Asked Questions

What should I do if my manufacturer says files are missing but I included everything?

First, verify your ZIP file actually contains all the files you think it does—occasionally files fail to add during compression. Check that none of your files are zero bytes (empty). If files are present and non-empty, the issue may be file recognition. Unclear naming can cause automated import systems to miss files. Ask your manufacturer which specific files they need, and either rename your files to match their expected naming convention or include a readme document mapping your file names to layer functions.

How do I fix drill files that show holes offset from pads?

Drill-to-pad misalignment almost always results from different coordinate origins between Gerber and drill exports. In your CAD software, ensure both exports use the same origin reference point (board origin, absolute origin, or aux axis origin—just make them match). Export both file types again with consistent settings. Before resubmitting, load the new files into a Gerber viewer and overlay the drill layer on a copper layer. Zoom in on several pads to verify holes are centered. If alignment is still off after matching origins, check for unit mismatches (inches vs. millimeters) which would cause 25.4x scaling errors.

Why does my solder mask appear inverted in the Gerber viewer?

Solder mask polarity confusion is common. The industry convention is “positive” polarity where drawn features in the Gerber file represent areas where mask will be removed (pad openings). If your viewer shows the entire board covered or entirely exposed, your CAD tool may have exported with inverted polarity. Check your export settings for a “negative” or “polarity” option and ensure it’s set for positive/normal output. Some Eagle versions default to negative polarity for solder mask—uncheck this option in the CAM Processor before export.

Can manufacturers fix minor Gerber errors, or do I need to regenerate files?

Many manufacturers can make minor corrections during their CAM review process, but this adds time and introduces risk. Issues like missing silkscreen layers, minor clearance violations, or silkscreen-on-pad problems can often be corrected. However, more significant problems—missing drill files, wrong formats, misaligned layers, incorrect outlines—require you to fix the source files and resubmit. Even when manufacturers can fix problems, they charge engineering fees for the time involved. Fixing errors yourself before submission is faster, cheaper, and ensures the corrections match your design intent.

What’s the difference between a drill file and a drill map?

A drill file contains NC (numerical control) code that directly programs drilling machines. It includes coordinate data for each hole location and tool definitions for each hole size. File extensions are typically .DRL, .XLN, or .NC. A drill map is a visual reference document showing hole locations and sizes in human-readable form—think of it as a diagram of your drill pattern. While useful for documentation, drill maps cannot be processed by manufacturing equipment. If your manufacturer requests a drill file and you provide a drill map, they cannot drill your board. When exporting from your CAD tool, select “Generate Drill File” or similar, not “Generate Drill Map” or “Generate Drill Drawing.”

Conclusion

Common Gerber file errors share one thing in common: they’re all preventable. Missing files result from incomplete checklists. Alignment errors come from inconsistent export settings. Format problems happen when export options aren’t verified. Every error in this guide can be caught before submission with systematic verification.

Build a personal verification routine: export your Gerbers, open them in a viewer, overlay all layers, verify alignment, run a DFM check, then submit. The few extra minutes this takes pays back in faster turnaround, fewer engineering questions, and boards that work correctly the first time.

When errors do slip through, respond quickly with corrected files. Provide context about what you changed so the manufacturer can verify the correction. And document what went wrong so you can add that specific check to your verification process for next time.

The goal isn’t perfection—it’s systematic improvement. Each error you catch teaches you what to check for, building toward a personal process that catches problems before they become expensive manufacturing delays.