How to Read and Verify Gerber Files Before Sending to Manufacture

Generating Gerber files from your EDA tool is not the last step — it is the second-to-last. Before you zip those files and upload them to a fabricator, you must open and inspect every layer. A five-minute Gerber review has saved countless makers from wasted boards, missed deadlines and unnecessary respins.

What Are Gerber Files?

Gerbers are the industry-standard format that tells a PCB manufacturer exactly where to etch copper, drill holes, apply solder mask and print silkscreen. A typical 2-layer export produces six to eight files:

• *.GTL — Top copper (F.Cu)
• *.GBL — Bottom copper (B.Cu)
• *.GTS — Top solder mask
• *.GBS — Bottom solder mask
• *.GTO — Top silkscreen
• *.GBO — Bottom silkscreen
• *.GKO / *.GM1 — Board outline (Edge.Cuts)
• *.DRL — Drill file (Excellon format)

Step 1: Open a Gerber Viewer

Do not rely on your EDA tool's built-in 3D preview — use a dedicated Gerber viewer that renders files exactly as the manufacturer will. Good free options:

• KiCad Gerber Viewer (built-in, offline) — File → Open Gerbers
• Tracespace.io — drag-and-drop, runs in your browser
• PCB LAB upload page — shows a rendered preview after you upload your zip

Step 2: Check the Board Outline

Load the edge-cuts / board outline layer first. Verify:

• The outline is a single closed polygon — no gaps, no duplicate lines.
• The board dimensions match what you intended.
• There are no stray lines outside the board boundary.

A broken outline is one of the most common reasons a fab rejects a Gerber package. Zoom into every corner and confirm the lines meet cleanly.

Step 3: Inspect Copper Layers

Load the top and bottom copper layers and check each one:

• All traces are routed — no unconnected ratsnest lines visible.
• Copper pours (ground planes) are present and connected to the net.
• No copper extends outside the board outline.
• Pad sizes match the component footprints you intended.

Step 4: Verify the Drill File

Load the drill file on top of the copper layers. Every drill hit should land in the centre of a pad or via annular ring. Watch for:

• Drill hits with no surrounding copper ring (via too close to edge, or footprint error).
• Missing drill file — without it, no holes are drilled and the board is useless.
• Drill sizes below the fab's minimum (PCB LAB minimum: 0.3 mm finished hole).

Step 5: Check Solder Mask Openings

The solder mask layer defines where the green lacquer is removed (i.e., where solder can stick). Load the mask layers and confirm:

• Every pad has a corresponding mask opening — you will see pads as "holes" in the mask layer.
• Mask openings are not larger than necessary; oversized openings can cause solder bridging.
• No mask openings in the middle of the board where there are no pads.

Step 6: Review the Silkscreen

The silkscreen prints component labels, polarity marks and board identifiers. Check:

• Reference designators (R1, C3, U1…) are legible and not overlapping pads.
• Polarity indicators (+ signs, pin-1 dots, diode bands) are correct.
• Text is above the fab's minimum size (PCB LAB minimum: 1 mm tall, 0.15 mm stroke).

Common Problems and Fixes

• Missing drill file — re-export; make sure Excellon drill is checked in plot settings.
• Open board outline — in KiCad, use Edit → Cleanup Graphics to merge segments.
• Copper outside outline — select and delete, or shrink the copper pour.
• Wrong Gerber units — PCB LAB accepts both mm and inches; confirm your export setting matches.