How to Generate Gerber Files in EasyEDA Standard Edition: Complete PCB Engineer’s Guide

You’ve spent hours perfecting your PCB layout in EasyEDA, routing traces, placing components, and checking your design. Now you’re ready for the moment that actually turns your digital design into physical hardware: generating Gerber files.

As someone who’s designed dozens of boards using EasyEDA Standard Edition, I can tell you that this browser-based tool makes Gerber generation remarkably simple compared to traditional desktop software. But there are still important details that can trip you up if you’re not careful. This guide walks you through the entire process, from pre-export checks to verification, ensuring your files are ready for any PCB manufacturer.

Understanding Gerber Files in EasyEDA

Before diving into the export process, let’s clarify what Gerber files actually are and why they matter. Gerber files (RS-274X format) are the industry-standard way to communicate PCB designs to manufacturers. They’re essentially 2D vector images that describe each layer of your board, from copper traces to solder mask to silkscreen.

EasyEDA generates Gerber files in RS-274X format, which embeds aperture information directly into the files. This is the modern standard that virtually all PCB fabricators accept. When you export from EasyEDA, you’re creating a complete manufacturing package that includes Gerber files for each layer plus Excellon drill files for all the holes in your board.

Gerber Files Generated by EasyEDA Standard Edition

File Name	Extension	Description
Gerber_TopLayer	.GTL	Top copper layer with traces and pads
Gerber_BottomLayer	.GBL	Bottom copper layer
Gerber_Inner1, Inner2…	.G1, .G2…	Inner copper layers (multilayer boards)
Gerber_TopSolderMaskLayer	.GTS	Top solder mask openings
Gerber_BottomSolderMaskLayer	.GBS	Bottom solder mask openings
Gerber_TopSilkscreenLayer	.GTO	Top silkscreen markings
Gerber_BottomSilkscreenLayer	.GBO	Bottom silkscreen markings
Gerber_TopPasteMaskLayer	.GTP	Top paste mask for stencils
Gerber_BottomPasteMaskLayer	.GBP	Bottom paste mask for stencils
Gerber_BoardOutlineLayer	.GKO	Board outline and cutouts
Drill_PTH_Through	.DRL	Plated through-hole drill file
Drill_NPTH_Through	.DRL	Non-plated through-hole drill file

Pre-Export Preparation: Essential Checks Before Generating Gerbers

Rushing straight to Gerber generation without proper preparation is a common mistake that leads to manufacturing delays, rejected files, or worse, boards that don’t work. Here’s what you need to check first.

Run Design Rule Check (DRC)

EasyEDA’s Design Rule Check is your first line of defense against manufacturing problems. The tool features real-time DRC that marks errors with an “X” flag as you design, but you should still run a full check before export.

To run DRC in EasyEDA Standard Edition:

1. Navigate to Tools → Design Rule… or right-click the canvas and select Design Rule…
2. Review and adjust your design rules if needed
3. Go to Design Manager → DRC Error or Top Menu → Design → Check DRC
4. Click the refresh icon to run the complete check
5. Address all errors before proceeding

The DRC checks for clearance violations between objects with different nets, track width violations, via diameter issues, and drill diameter problems. If your PCB includes copper areas, the DRC may take longer to complete, so be patient with larger designs.

Verify Your Design Rules Match Manufacturer Capabilities

EasyEDA’s default design rules are configured to work with most manufacturers, including JLCPCB. However, if you’re using a different fabricator or have specific requirements, verify your rules match their capabilities.

Design Parameter	JLCPCB Minimum	EasyEDA Default	Recommended
Minimum Track Width	0.127mm (5mil)	0.254mm	0.2mm or higher
Minimum Clearance	0.127mm (5mil)	0.254mm	0.2mm or higher
Minimum Via Diameter	0.4mm	0.6mm	0.5mm or higher
Minimum Via Drill	0.2mm	0.3mm	0.3mm or higher
Minimum Hole Size	0.2mm	—	0.3mm or higher

Setting your clearances slightly higher than the manufacturer’s minimum gives you a safety margin and often results in faster, cheaper fabrication.

Rebuild Copper Areas

If you’ve made any changes to your design since last filling your copper pours, you need to rebuild them before generating Gerbers. Outdated copper fills won’t show in your Gerber output, potentially causing shorts or opens in your manufactured board.

Press Shift+B to rebuild all copper areas, or right-click on a copper area and select Rebuild Copper Area. Always verify the copper fill looks correct in your design before exporting.

Check Board Outline

Your board outline (Edge.Cuts layer in some tools, part of the BoardOutlineLayer in EasyEDA) must form a completely closed shape. Any gaps in the outline will cause your manufacturer to reject the files or make assumptions about your board shape.

Zoom in on corners and verify the outline is continuous. Slots and cutouts drawn using the solid region tool (Type: NPTH) will appear in the board outline file after Gerber generation.

Step-by-Step Guide to Generate Gerber Files in EasyEDA Standard Edition

With your design verified and ready, let’s walk through the Gerber generation process.

Step 1: Access the Gerber Generation Dialog

There are multiple ways to open the Gerber export dialog in EasyEDA Standard Edition:

Method 1 (Menu): Navigate to File → Generate PCB Fabrication File(Gerber)

Method 2 (Alternative Menu): Go to Fabrication → PCB Fabrication File(Gerber)

Method 3 (Toolbar): Click the Generate Gerber button in the top toolbar (folder icon with “G”)

Any of these methods opens the Gerber generation dialog where you’ll configure and export your files.

Step 2: Review the Gerber Preview

When the dialog opens, you’ll see a preview image of your PCB along with manufacturing parameters. Take a moment to verify:

• The board dimensions look correct
• All layers are represented
• The board outline is closed and accurate
• No obvious missing features

This preview gives you a quick sanity check before committing to the export.

Step 3: Configure Export Options

EasyEDA Standard Edition uses sensible defaults for Gerber generation, but you should understand the key settings:

Drill File Coordinate Format: The default is 3:3 (three integer digits, three decimal digits). This works for most boards. For very large PCBs exceeding the coordinate range, EasyEDA automatically switches to 4:2 format.

Gerber Format: EasyEDA generates RS-274X format, which is universally compatible. The aperture information is embedded in the files.

Coordinate Origin: Gerber file coordinates follow the canvas coordinates in your design. Keep this in mind if you need specific positioning for panelization.

Step 4: Generate the Gerber Files

Click the Generate Gerber button at the bottom of the dialog. EasyEDA will process your design and create a compressed ZIP archive containing all the necessary manufacturing files.

Important: The Gerber files are generated by your browser, so you must use your browser’s built-in download function to save them. Third-party download managers may not work correctly.

The ZIP file will download to your default downloads folder. The filename typically includes your project name for easy identification.

Step 5: Verify File Contents

After downloading, unzip the archive and verify all expected files are present:

• Copper layer files (.GTL, .GBL, and inner layers if applicable)
• Solder mask files (.GTS, .GBS)
• Silkscreen files (.GTO, .GBO)
• Paste mask files (.GTP, .GBP) if your design has SMD components
• Board outline file (.GKO)
• Drill files (.DRL) for PTH and NPTH holes

Missing files usually indicate missing features in your design. For example, if there’s no bottom silkscreen file, your design likely has no silkscreen on the bottom layer.

Understanding EasyEDA Gerber File Contents

Let me break down what each file in your Gerber package actually contains, so you know what to look for when verifying.

Copper Layer Files (GTL, GBL, G1, G2…)

These files contain all the copper features on each layer: traces, pads, vias, and copper pours. The top copper is .GTL (Gerber Top Layer), bottom is .GBL (Gerber Bottom Layer), and inner layers are numbered .G1, .G2, etc.

Solder Mask Files (GTS, GBS)

Solder mask files define where the mask should NOT be applied, exposing copper for soldering. These files show openings over pads, vias (if not tented), and any other areas where you need bare copper.

Silkscreen Files (GTO, GBO)

Silkscreen layers contain component outlines, reference designators, logos, and other markings printed on your board. The top silkscreen is .GTO, bottom is .GBO.

Paste Mask Files (GTP, GBP)

These files define stencil openings for solder paste application during SMT assembly. Only SMD pads appear in paste mask files. If you’re not doing assembly or using through-hole only, these files may be empty or omitted.

Board Outline File (GKO)

The board outline file defines the physical shape of your PCB. The manufacturer uses this to route (cut) your board from the panel. It includes the outer boundary plus any internal cutouts or slots.

Drill Files (DRL)

EasyEDA generates separate drill files for plated through-holes (PTH) and non-plated through-holes (NPTH). PTH includes vias and component holes that need copper plating. NPTH includes mounting holes and slots that should not be plated.

Assembly and Documentation Files

EasyEDA also generates additional files that don’t affect manufacturing but provide useful information:

File	Extension	Purpose
Gerber_TopAssemblyLayer	.GTA	Top assembly drawing (reference only)
Gerber_BottomAssemblyLayer	.GBA	Bottom assembly drawing (reference only)
Gerber_MechanicalLayer	.GML	Mechanical notes, V-cut paths (reference only)
Gerber_DocumentLayer	.GDL	Documentation notes (reference only)

Verifying Your EasyEDA Gerber Files

Never send Gerber files to a manufacturer without verification. A few minutes of checking can save days of delays and wasted money.

Using EasyEDA’s Built-in Gerber Viewer

EasyEDA provides an online Gerber viewer that’s perfect for quick verification. In the Gerber generation dialog, click Gerber View to open your files in the viewer. You can also access the viewer directly at https://easyeda.com/GerberViewer.

The EasyEDA Gerber Viewer provides:

• Layer-by-layer viewing with toggles
• Top and bottom photo-realistic views
• Basic DFM (Design for Manufacturability) analysis
• Board dimension detection
• Drill hole information

Third-Party Gerber Viewers

For more thorough verification, especially if you’re using a manufacturer other than JLCPCB, consider these free Gerber viewers:

Tool	Platform	Features	Download
Gerbv	Windows/Linux/Mac	Open source, measurements, PNG export	gerbv.github.io
ViewMate	Windows	Professional features, user-friendly	pentalogix.com
FlatCAM	Windows/Linux/Mac	Gerber editing, CNC output	flatcam.org
CAM350	Windows	Industry standard (paid, free viewer)	Professional tool
GerberLogix	Windows	Free for non-commercial use	easylogix.de

Verification Checklist

Before ordering, systematically check:

• All copper layers show correct traces and pads
• No missing or broken traces
• Drill holes align with pad centers
• Via drill sizes are appropriate
• Solder mask exposes all pads correctly
• Silkscreen doesn’t overlap pads
• Board outline is closed and correct size
• All cutouts and slots appear correctly
• Component footprints match your actual components

Ordering PCBs Directly from EasyEDA

One of EasyEDA’s biggest advantages is its seamless integration with JLCPCB for ordering. Since EasyEDA is owned by JLCPCB, the workflow is optimized for direct ordering.

Direct Order Process

Instead of clicking “Generate Gerber,” you can click Save to Cart in the Gerber dialog. This:

1. Automatically uploads your Gerber files to JLCPCB
2. Runs their automated DFM check
3. Calculates pricing based on your board specifications
4. Adds the order to your JLCPCB cart

You’ll see real-time pricing as you adjust parameters like quantity, color, thickness, and finish.

Using Gerbers with Other Manufacturers

If you prefer a different manufacturer, simply download the Gerber ZIP file and upload it to your chosen fabricator’s website. EasyEDA’s Gerber output is industry-standard RS-274X format, compatible with virtually any PCB manufacturer worldwide.

Popular alternatives include:

• PCBWay
• OSH Park
• Seeed Studio Fusion
• AllPCB
• Elecrow

Each manufacturer has their own upload portal and may run additional DFM checks on your files.

Common EasyEDA Gerber Generation Issues and Solutions

Even with EasyEDA’s streamlined process, issues can occur. Here are the problems I encounter most frequently and how to solve them.

Drill Holes Appear Offset in Viewer

Symptom: When viewing Gerbers in tools like CAM350, drill holes don’t align with pads.

Cause: Coordinate format mismatch between the Gerber files and your viewer settings.

Solution: In your Gerber viewing tool, set the drill file coordinate format to 3:3 (mm) or 2:4 (inches) to match EasyEDA’s output. EasyEDA defaults to 3:3 format for standard-sized boards.

Cannot Find Generate Gerber Option

Symptom: The Gerber generation menu item is missing or grayed out.

Cause: You’re likely in the Footprint Editor or Schematic Editor instead of the PCB Editor. Gerbers can only be generated from PCB designs.

Solution: Open your PCB file (not schematic or footprint) in the PCB Editor. The Gerber generation option is only available when editing a PCB document.

DRC Errors Blocking Export

Symptom: EasyEDA prompts about DRC errors when you try to generate Gerbers.

Cause: Your design has unresolved design rule violations.

Solution: Click “Yes” to review the errors, or “No” to continue with export despite errors. While you can generate Gerbers with DRC errors, doing so risks manufacturing problems. Fix all errors for production-quality boards.

Missing Copper Pour in Gerber Output

Symptom: Copper areas that appear in your design are missing from the Gerber files.

Cause: Copper areas weren’t rebuilt after design changes.

Solution: Press Shift+B to rebuild all copper areas before generating Gerbers. If the option “Check Object to Copper Area” is disabled in DRC settings, copper areas may not update automatically.

Download Fails or File is Corrupt

Symptom: The Gerber ZIP file won’t download or can’t be extracted.

Cause: Third-party download managers interfering with browser-generated files.

Solution: Use your browser’s built-in download function only. Disable download managers temporarily if needed. Try a different browser (Chrome typically works best with EasyEDA).

Flying Leads Warning

Symptom: EasyEDA warns about flying leads when generating Gerbers.

Cause: Unconnected nets exist in your PCB design.

Solution: Click “Yes” to locate and review unconnected nets, or “No” to ignore and continue. Flying leads often indicate incomplete routing that should be addressed before manufacturing.

Useful Resources for EasyEDA Gerber Generation

Official Documentation and Tools

• EasyEDA Standard Documentation: https://docs.easyeda.com — Complete user guide
• EasyEDA Online Gerber Viewer: https://easyeda.com/GerberViewer — Built-in verification tool
• JLCPCB Capabilities: https://jlcpcb.com/capabilities — Manufacturing specifications
• EasyEDA Forum: https://easyeda.com/forum — Community support

Free Gerber Viewers

• Gerbv: https://gerbv.github.io — Open source, cross-platform
• Gerbv SourceForge: https://sourceforge.net/projects/gerbv — Windows download
• FlatCAM: http://flatcam.org — Gerber editing and CNC output
• ViewMate: https://www.pentalogix.com — Professional free viewer

Gerber Format Specification

• Ucamco Gerber Format: https://www.ucamco.com/gerber — Official RS-274X specification

Frequently Asked Questions

Can I use EasyEDA Gerber files with any PCB manufacturer?

Yes, EasyEDA generates industry-standard RS-274X Gerber files that are compatible with virtually all PCB manufacturers worldwide. While EasyEDA integrates seamlessly with JLCPCB, you can download the Gerber ZIP file and upload it to PCBWay, OSH Park, Seeed Studio, or any other fabricator. The files include all necessary layers and drill information in universally accepted formats.

Why does EasyEDA generate separate PTH and NPTH drill files?

Plated through-holes (PTH) and non-plated through-holes (NPTH) require different manufacturing processes. PTH holes like vias and component leads need copper plating on the inner walls to create electrical connections between layers. NPTH holes like mounting holes shouldn’t have plating. Keeping them separate gives manufacturers clear instructions about which holes need plating. Most manufacturers accept merged drill files too, but separate files reduce the chance of errors.

What should I do if my Gerber viewer shows misaligned drill holes?

This is almost always a coordinate format mismatch. EasyEDA defaults to 3:3 format (three integer digits, three decimal digits) for the drill file. In your Gerber viewer’s settings, ensure the drill file import format matches. In Gerbv, this is set when opening the file. In CAM350, check the drill file import settings. Try different format combinations (3:3, 2:4, 4:2) until the holes align with pads.

How do I generate Gerbers for a multilayer PCB in EasyEDA?

The process is identical to two-layer boards. When you generate Gerbers, EasyEDA automatically includes all copper layers in your design. For a 4-layer board, you’ll get GTL (top), G1 (inner 1), G2 (inner 2), and GBL (bottom) copper files, plus all the standard mask, silkscreen, and drill files. Verify in your Gerber viewer that all inner layers contain the expected routing and planes.

Can I edit Gerber files after exporting from EasyEDA?

EasyEDA does not support importing or editing Gerber files directly. If you need to make changes, you must edit your PCB design in the EasyEDA editor and regenerate the Gerbers. While some professional CAM tools like CAM350 or ViewMate Deluxe can edit Gerbers, this is generally not recommended. Editing Gerbers directly can introduce errors and breaks the link between your design files and manufacturing files. Always make changes in your source PCB design.

Final Thoughts

Generating Gerber files in EasyEDA Standard Edition is straightforward once you understand the workflow. The key steps are: verify your design with DRC, rebuild copper areas, generate the Gerber package, and verify the output before ordering.

What makes EasyEDA particularly appealing is the tight integration with JLCPCB. You can go from completed design to ordered PCBs in literally three clicks. But even if you’re using a different manufacturer, EasyEDA’s standard RS-274X output works everywhere.

The most important advice I can give: never skip verification. Load your Gerbers into a viewer, check every layer, verify drill alignment, and confirm your board outline is correct. Those few minutes of checking are worth far more than the time and money lost to a bad board order.