Notes for Gerber Files Generated from Specific Versions: Eagle 9.x and KiCad 7/8/9

Every PCB designer knows the frustration of submitting Gerber files only to receive a message from the manufacturer asking for corrections. The problem often traces back to version-specific export quirks in your CAD software. Eagle 9.x and KiCad 7/8/9 each have particular settings, default behaviors, and known issues that can cause manufacturing problems if you’re not aware of them. This guide documents the critical notes, settings, and workarounds for generating clean Gerber files from these popular PCB design tools.

Why Version-Specific Gerber Notes Matter

Gerber export functions change between software versions. What worked in Eagle 8 may produce different results in Eagle 9. KiCad 7’s default settings differ from KiCad 8 and 9. Manufacturers receive thousands of Gerber packages weekly, and files with subtle export errors create delays, extra engineering questions, and sometimes costly respins.

Common Version-Related Issues

Issue Category	Eagle 9.x Impact	KiCad 7/8/9 Impact
Format compatibility	RS-274X vs X2 confusion	X2 attributes causing import errors
Missing layers	Bottom silkscreen not exported by default	NPTH drill files generated separately
Board outline	Milling layer (46) often omitted	Edge.Cuts layer gaps cause rejection
Drill files	Coordinate format inconsistencies	PTH/NPTH merge options changed
Naming conventions	Non-standard extensions confuse fab	Protel extensions require explicit enable

Understanding these version-specific behaviors prevents manufacturing delays and ensures your boards come back exactly as designed.

Eagle 9.x Gerber Export Notes

Eagle 9.x introduced significant changes to the CAM Processor interface compared to earlier versions. Autodesk continues updating Eagle frequently, and each point release can introduce subtle differences in export behavior.

CAM Processor Changes in Eagle 9.x

The CAM Processor in Eagle 9.x works differently than versions 7 and 8. The interface changed substantially, and some legacy CAM job files require modification to work correctly.

Eagle Version	CAM Processor Behavior
Eagle 7.x	Separate gerb274x.cam and excellon.cam files
Eagle 8.x	Combined CAM jobs, legacy interface
Eagle 9.0-9.1	New interface, compatibility issues with legacy jobs
Eagle 9.2+	Built-in Gerber preview, automatic ZIP output
Eagle 9.6+	Improved example CAM jobs, template system

Key change: Eagle 9.x versions automatically package output files into a ZIP archive. Earlier versions required manual file collection.

Critical Settings for Eagle 9.20 and Later

Eagle 9.20 introduced new default settings that can cause manufacturing problems if not corrected before export.

Solder Mask Negative Polarity Issue

When opening the CAM Processor in Eagle 9.20+, the solder mask layers have “Negative Polarity” checked by default. This setting must be unchecked for correct output, otherwise the solder mask Gerber files will be inverted—pads covered instead of exposed.

Profile Layer Configuration

The board outline requires both the Dimension layer (20) and Milling layer (46) for complete output. Many CAM job files only include Dimension, missing cutouts and slots defined on the Milling layer.

Layer	Purpose	Must Include
20 Dimension	Board outline, external edges	Always
46 Milling	Internal cutouts, slots, v-cuts	If present in design

Multilayer Drill File Generation

For boards with more than 4 layers containing blind or buried vias, Eagle 9.x requires explicit drill file generation based on the PCB stackup:

1. Right-click on Drill → Excellon in the CAM Processor
2. Select “Generate Excellon outputs based on PCB stackup”
3. Process Job to generate all required drill files

Eagle 9.x Layer Mapping for Gerber Export

Eagle Layer	Gerber Purpose	Protel Extension
1 Top	Top copper	.GTL
16 Bottom	Bottom copper	.GBL
29 tStop	Top solder mask	.GTS
30 bStop	Bottom solder mask	.GBS
21 tPlace + 25 tNames	Top silkscreen	.GTO
22 bPlace + 26 bNames	Bottom silkscreen	.GBO
20 Dimension + 46 Milling	Board outline	.GKO
Drills + Holes	Drill data	.XLN or .DRL

Bottom Silkscreen Export Issue

Eagle’s default CAM jobs only export top silkscreen (tPlace and tNames layers). If your board has bottom silkscreen, you must manually add the bottom silkscreen output:

1. In CAM Processor, click “Add” to create a new section
2. Name it “Silkscreen Bottom” or similar
3. Set filename to “%N.GBO” (using Protel extension)
4. Select layers: 20 Dimension, 22 bPlace, 26 bNames
5. Deselect all other layers

Eagle 9.x RS-274X vs X2 Format Issues

Some Eagle 9.x versions output Gerber X2 format even when RS-274X is specified. This causes compatibility problems with manufacturers whose CAM software doesn’t support X2 headers.

Workaround options:

Use legacy CAM job files from Eagle 8.5.2 without modification. The older format CAM jobs produce clean RS-274X output.

Manually edit exported Gerber files to remove X2 header lines (lines starting with %TF, %TA, %TO) if your manufacturer rejects them.

Eagle 9.x Slot and Cutout Handling

Eagle doesn’t support slots directly in the same way as other CAD tools. Slots appear in different ways depending on how they were created:

Slot Type	Eagle Layer	Export Behavior
Milled slots (non-plated)	Layer 46 Milling	Merged into outline (.GKO)
Plated slots	Copper layers + Drills	Merged into drill file (.XLN)
V-cuts	Layer 46 Milling	Included in outline layer

Minimum plated slot width is typically 0.65mm (25.6 mils). Ensure your CAM job includes both Dimension and Milling layers in the outline output.

KiCad 7 Gerber Export Notes

KiCad 7 established the modern Gerber export workflow that continues through versions 8 and 9. Understanding version 7’s behavior provides the foundation for working with all recent KiCad releases.

KiCad 7 Plot Settings for Manufacturing

Access Gerber export through File → Fabrication Outputs → Gerbers (.gbr). The default settings in KiCad 7 are NOT suitable for most manufacturers without adjustment.

Required Settings Changes for KiCad 7:

Setting	Default	Recommended
Use Protel filename extensions	Unchecked	Checked
Subtract soldermask from silkscreen	Unchecked	Checked
Plot reference designators	Unchecked	Checked
Check zone fills before plotting	Unchecked	Checked
Use extended X2 format	Checked	Depends on manufacturer

Important: Many Chinese PCB manufacturers (JLCPCB, PCBWay, etc.) prefer RS-274X format and may have issues with X2 attributes. If in doubt, uncheck “Use extended X2 format.”

KiCad 7 Required Layers for Export

KiCad Layer	Function	Protel Extension
F.Cu	Front copper	.GTL
B.Cu	Back copper	.GBL
F.Silkscreen	Front silkscreen	.GTO
B.Silkscreen	Back silkscreen	.GBO
F.Mask	Front solder mask	.GTS
B.Mask	Back solder mask	.GBS
Edge.Cuts	Board outline	.GKO
In1.Cu, In2.Cu…	Inner layers (if applicable)	.G2, .G3…

KiCad 7 Drill File Generation

After generating Gerber files, click “Generate Drill Files…” in the same Plot window. Critical settings:

Setting	Recommended Value
Drill Units	Millimeters (preferred) or Inches
Zeros Format	Decimal format
Drill Origin	Absolute or Drill/place file origin
Drill File Format	Excellon
PTH and NPTH in single file	Check for simplicity
Oval Holes Drill Mode	Use alternate drill mode

PTH/NPTH Note: KiCad 7 may generate separate PTH (plated through-hole) and NPTH (non-plated through-hole) drill files. If your manufacturer prefers merged files, check “PTH and NPTH in single file” to avoid missing holes.

KiCad 8 Gerber Export Notes

KiCad 8 refined the export interface and changed some default behaviors from version 7. Most settings remain similar, but several options moved or changed names.

KiCad 8 Interface Changes

The Plot dialog in KiCad 8 reorganized options for better clarity. Key functional changes:

Feature	KiCad 7	KiCad 8
Gerber preview	Limited	Improved built-in viewer
Zone fill check	Manual enable	More prominent warning
Drill file button	Same window	Same window, clearer layout
X2 format option	General Options	Gerber Options section

KiCad 8 Specific Considerations

Zone Fill Warning

KiCad 8 more aggressively warns about outdated zone fills. When “Check zone fills before plotting” is enabled and fills are stale, KiCad prompts for confirmation before regenerating. Always click “Refill” to ensure copper pours reflect your current design.

Aperture Macro Support

KiCad 8 uses aperture macros for complex pad shapes. Some older CAM software has issues with these macros. If you experience problems with hexagonal pads, custom pad shapes, or thermal reliefs not displaying correctly:

1. Check “Disable aperture macros” in the Gerber Options
2. This increases file size but improves compatibility
3. Only use this option if experiencing specific problems

Gerber X2 Slot Definition Issue

A known issue in KiCad 8 (and earlier versions) involves slot holes in Gerber X2 format drill files. KiCad uses obround apertures with Flash commands for slots, which technically violates the Gerber specification. Most manufacturers handle this correctly, but if you encounter slot problems:

• Use Excellon format for drill files instead of Gerber X2
• Or regenerate drill files with “PTH and NPTH in single file” checked

KiCad 9 Gerber Export Notes

KiCad 9 introduced further refinements to the export workflow, with some options renamed or relocated compared to version 8.

KiCad 9 Interface Changes from Version 8

Users upgrading from KiCad 8 to 9 notice several changes in the Gerber generation dialog:

Change	KiCad 8 Location	KiCad 9 Status
Global solder mask minimum	Board Setup	Warning displayed during plot
Tent vias option	Plot dialog	Moved/renamed
Plot footprint values	General Options	Reorganized
Plot footprint text	Separate option	Combined options

Adaptation tip: If following manufacturer guides written for KiCad 8, expect minor differences in option locations. The underlying functionality remains the same—just look for similarly named options in the reorganized interface.

KiCad 9 Recommended Export Settings

Setting Category	Option	Recommended
Plot format	Gerber	Yes (default)
Output directory	Your choice	Create dedicated folder
Include Layers	All fabrication layers	Select appropriately
General Options	Plot reference designators	Checked
General Options	Use drill/place file origin	Checked
General Options	Check zone fills before plotting	Checked
Gerber Options	Use Protel filename extensions	Checked
Gerber Options	Subtract soldermask from silkscreen	Checked
Gerber Options	Use extended X2 format	Manufacturer dependent
Gerber Options	Disable aperture macros	Only if needed

KiCad 9 Drill File Best Practices

KiCad 9 maintains the same drill file generation workflow as versions 7 and 8. Generate drill files from within the Plot dialog by clicking “Generate Drill Files…”

Recommended drill settings for KiCad 9:

• Format: Excellon (most compatible)
• Drill Units: Millimeters
• Zeros Format: Decimal format
• Map File Format: Gerber (optional, for reference)
• PTH and NPTH: Single file unless manufacturer specifies otherwise

Common Issues Across Both Tools

Certain Gerber export problems appear regardless of whether you’re using Eagle or KiCad. Awareness of these issues helps catch problems before submission.

Board Outline Problems

Problem	Eagle Solution	KiCad Solution
Missing outline	Include layers 20 + 46	Verify Edge.Cuts is selected
Gaps in outline	Check wire connections	Ensure closed shape
Outline on wrong layer	Use Dimension layer	Use only Edge.Cuts
Missing cutouts	Add Milling layer to output	Draw cutouts on Edge.Cuts

Drill Alignment Issues

Both tools can produce drill files that don’t align with copper layers if coordinate settings differ between outputs.

Prevention checklist:

• Use consistent units (mm or inches) across all outputs
• Use the same origin reference for Gerber and drill files
• Verify coordinate format matches between copper and drill exports
• Check zero suppression settings match manufacturer requirements

File Naming for Manufacturer Compatibility

Standard Protel extensions improve automated layer recognition at PCB factories.

Layer Function	Protel Extension	Eagle Default	KiCad Default
Top Copper	.GTL	.cmp	-F_Cu.gbr
Bottom Copper	.GBL	.sol	-B_Cu.gbr
Top Mask	.GTS	.stc	-F_Mask.gbr
Bottom Mask	.GBS	.sts	-B_Mask.gbr
Top Silk	.GTO	.plc	-F_Silkscreen.gbr
Bottom Silk	.GBO	.pls	-B_Silkscreen.gbr
Outline	.GKO	.gko	-Edge_Cuts.gbr
Drill	.DRL or .XLN	.drl	.drl

Enable Protel extensions in both tools to avoid layer identification confusion at the manufacturer.

Useful Resources

Eagle 9.x Resources

Resource	URL	Description
JLCPCB Eagle CAM Files	jlcpcb.com/help/article/137	Predefined CAM jobs for Eagle
PCBWay Eagle Guide	pcbway.com/helpcenter/generate_gerber	Version-specific tutorials
Seeed Studio CAM Files	seeedstudio.com/blog	Updated CAM files for 9.4.2+
Autodesk Eagle Forums	forums.autodesk.com/t5/eagle-forum	Community support

KiCad 7/8/9 Resources

Resource	URL	Description
KiCad Official Documentation	docs.kicad.org	Version-specific guides
JLCPCB KiCad Guides	jlcpcb.com/help	KiCad 7, 8, 9 tutorials
PCBWay KiCad Tutorials	pcbway.com/helpcenter/generate_gerber	Export walkthroughs
KiCad Forums	forum.kicad.info	Community support
OSH Park KiCad Guide	docs.oshpark.com/design-tools/kicad	Manufacturer-specific settings

Gerber Viewers for Verification

Tool	Platform	URL
KiCad GerbView	All	Included with KiCad
Gerbv	All	gerbv.github.io
ViewMate	Windows	pentalogix.com
JLCPCB Gerber Viewer	Online	jlcpcb.com
PCBWay Gerber Viewer	Online	pcbway.com

Frequently Asked Questions

Why does my manufacturer reject Gerber X2 files from KiCad?

Some manufacturers’ CAM software doesn’t fully support Gerber X2 attributes, particularly the %TF (file attributes) and %TA (aperture attributes) headers. While X2 is the newer standard with useful metadata, compatibility varies. If your manufacturer reports parsing errors or layer identification problems with X2 files, regenerate with “Use extended X2 format” unchecked in KiCad’s Plot settings. This produces RS-274X format files that virtually all CAM systems accept. Eagle 9.x users experiencing similar issues should use legacy CAM job files from version 8.5.2.

How do I fix the negative polarity solder mask issue in Eagle 9.20?

Eagle 9.20 and later versions default to “Negative Polarity” checked for solder mask layers in the CAM Processor. This inverts the mask, covering pads instead of exposing them. Before processing your job, expand the solder mask section in the CAM Processor and uncheck “Negative Polarity” for both top and bottom solder mask outputs. Alternatively, download manufacturer-provided CAM job files that have this setting correctly configured. Always verify solder mask layers in a Gerber viewer before submission—pads should appear as openings (exposed areas) in the mask.

Why are my KiCad drill holes in a separate NPTH file?

KiCad generates separate files for plated through-holes (PTH) and non-plated through-holes (NPTH) by default. This separation is technically correct since these holes require different manufacturing processes. However, some manufacturers prefer merged files, and having separate files increases the risk of forgetting to include the NPTH file. To merge them, check “PTH and NPTH in single file” in the Generate Drill Files dialog. If you’re using footprints imported from other sources, verify their hole definitions—mounting hole footprints sometimes incorrectly specify NPTH when they should be PTH, causing unexpected file separation.

What layers must I include for a complete Eagle 9.x Gerber package?

A complete Eagle 9.x Gerber package for a two-layer board requires these outputs: Top Copper (layer 1), Bottom Copper (layer 16), Top Solder Mask (layer 29 tStop), Bottom Solder Mask (layer 30 bStop), Top Silkscreen (layers 21 tPlace + 25 tNames + 20 Dimension), Board Outline (layers 20 Dimension + 46 Milling), and Drill File (Drills + Holes layers). If your board has bottom silkscreen, manually add that output including layers 22 bPlace + 26 bNames + 20 Dimension. For multilayer boards, add inner copper layers and potentially multiple drill files for blind/buried vias. Always verify against your manufacturer’s specific requirements.

How do I handle slots and cutouts in KiCad 7/8/9?

Internal cutouts and board edge features go on the Edge.Cuts layer in KiCad. Draw cutouts as closed shapes (rectangles, polygons, or connected line segments) on Edge.Cuts—the Gerber export includes them automatically with the board outline. For slot holes in components, KiCad handles these through the footprint definition as obround or slot-type pads, which export to the drill file. If you’re creating custom slots, define them in the footprint using the appropriate pad type rather than drawing on Edge.Cuts, which would create a routed cutout rather than a drilled slot. Verify slot dimensions meet your manufacturer’s minimum requirements (typically 0.5-0.65mm width for plated slots).

Conclusion

Generating clean Gerber files from Eagle 9.x and KiCad 7/8/9 requires attention to version-specific settings and behaviors. Eagle users must watch for the negative polarity default in version 9.20+, ensure milling layers are included in outline output, and manually add bottom silkscreen when needed. KiCad users should enable Protel filename extensions, decide on X2 format based on manufacturer support, and verify PTH/NPTH drill file handling.

Before every submission, verify your Gerber package in a standalone viewer. Check that copper layers show expected traces and pads, solder masks expose the correct areas, silkscreen text is readable and not overlapping pads, the board outline is closed without gaps, and drill holes align with pad centers.

The few minutes spent understanding your CAD tool’s export quirks pays dividends in faster turnaround, fewer engineering questions, and boards that work correctly the first time.