Checking Gerber files is the bridge between PCB layout and a manufacturing order. Your board may pass electrical DRC inside the EDA tool, but DRC does not always prove that the exported package is complete. Errors can be introduced during plotting, drill generation, file naming, ZIP creation, or last-minute output-job changes.
A viewer inspection catches a different class of problems: missing outline files, shifted drill hits, bottom layers that were mirrored incorrectly, silkscreen printed over pads, or a solder mask layer that does not match the copper. These issues are often obvious when you look at the final files, and difficult to see if you only review the design database.
Start by loading the finished archive in the free Gerber viewer. If you are not sure whether the archive is complete, compare it with the PCB Gerber file checklist before you upload it to a manufacturer.
Quick answer
Open the final Gerber ZIP in a viewer, toggle layers one by one, overlay drills with copper, confirm the outline and board size, check bottom-side orientation, inspect mask and silkscreen clearances, and compare the result against your intended PCB before ordering.
Why visual inspection catches export mistakes
EDA design-rule checks evaluate the board database before CAM output. They are essential for spacing, net connectivity, annular ring rules, differential pair constraints, copper pours, and many electrical conditions. They do not always know that you forgot to select the bottom solder mask in a plot dialog, generated drills from a different origin, or zipped a folder that still contains last week's outline file.
Gerber inspection evaluates the files after export. That matters because the manufacturer does not build from the schematic, layout editor, or screenshot. The CAM operator imports Gerber image layers and drill data, then runs a DFM process against those files. Looking at the same data before upload reduces avoidable back-and-forth and helps you catch errors while the design intent is still fresh.
Step-by-step Gerber error check
- Load the final ZIP. Use the archive that will be sent to the fab, not a working folder. This confirms that required files are actually included and that no stale outputs are hiding beside the new ones.
- Identify every layer. Confirm top copper, bottom copper, solder mask layers, silkscreen layers if used, board outline, and drill files. For stencil or assembly work, also confirm paste layers. If file names are unclear, use the rendered content to identify what each layer represents.
- Toggle layers one by one. Empty layers, unexpected artwork, or duplicate-looking files are warning signs. Copper layers should show tracks, pads, pours, and clearances. Mask layers should show openings where solderable copper is exposed. Silkscreen should show reference designators and legends only where printing is wanted.
- Check registration and alignment. Overlay top copper, bottom copper, solder mask, outline, and drills. Holes should land in pads and vias. Mask openings should expose pads without uncovering unrelated copper. The outline should surround the routed board without unexpected offsets.
- Confirm the board outline. The profile should be closed and should match the intended finished size. Check internal cutouts, slots, panel tabs, castellations, and non-rectangular shapes. A missing or open outline is one of the most common reasons a fab asks for clarification.
- Check bottom-side mirroring. Bottom copper, bottom mask, and bottom silkscreen should align with the same drill and outline coordinate system. Do not judge a bottom text layer by readability alone; compare it with component orientation and pads.
- Look for missing layers. For a normal solder-masked two-layer board, a missing bottom mask is a red flag unless it was intentionally omitted, and a board outline is always required. Drill files are required whenever the design has drilled or routed features — vias, through-hole pads, slots, or mounting holes (a board with no holes can legitimately ship without one). A four-layer board should include internal copper layers in the intended order, plus stackup notes if the order depends on dielectric spacing or impedance.
- Inspect silkscreen clipping. Reference designators, polarity marks, and logos should not overlap pads, exposed copper, or the routed edge. If silk is clipped by the fab, markings can become misleading or disappear.
- Verify drill-to-copper relationship. Drill hits should be centered well enough to leave the annular ring required by your manufacturer. For fine-pitch vias or small through-hole pads, compare drill size, pad size, and fab capability instead of assuming a generic minimum.
- Compare against design intent. Review connectors, mounting holes, polarity marks, fiducials, test pads, antennas, keepout areas, and high-current traces. A viewer cannot know your intent, so this human comparison is still necessary.
Common Gerber errors in a viewer
| Common Gerber error | What it looks like in a viewer | Likely cause |
|---|---|---|
| Missing board outline | Copper and mask appear, but no routed perimeter is visible. | Outline layer was not plotted or was drawn on the wrong layer. |
| Shifted drill file | Holes are offset from pads by a consistent distance. | Different Gerber and drill origins, units, or coordinate formats. |
| Wrong bottom orientation | Bottom artwork does not align logically with pads or outline. | Manual mirroring or incorrect CAM export settings. |
| Silkscreen over pads | Text or logos overlap exposed copper or component pads. | Silk clearance rules were disabled or not checked after placement. |
| Missing apertures or empty draws | Pads, tracks, pours, or entire layers fail to render. | Unsupported or incomplete CAM output, or stale non-RS-274X files. |
| Old file in ZIP | One layer has a different outline, date, or geometry than others. | Exported into a reused folder and zipped old files with new ones. |
The three-layer safety net
A reliable pre-order process uses three checks. First, run EDA DRC with rules that match your selected manufacturer and technology level. Second, inspect the exported Gerber and drill ZIP visually. Third, read the manufacturer's DFM report or CAM feedback carefully. Many fabs run a DFM check before production, and that report can catch process-specific problems such as solder mask slivers, small annular rings, copper too close to the edge, or drill sizes outside the selected service.
These checks are not redundant. DRC knows design intent and net rules. The viewer shows export reality. The fab's DFM report applies the manufacturer's equipment, stackup, plating, etching, and assembly rules. When all three agree, the order is much less likely to be delayed by avoidable CAM questions.
Check it in the viewer before ordering
Load the ZIP in the Gerber viewer and work through the layers slowly. For a complete list of files needed for fabrication and assembly, use what files to send to a PCB manufacturer. That guide helps separate Gerbers and Excellon drills from BOM, centroid, assembly drawing, and other PCBA deliverables.
FAQ
- Can a Gerber viewer replace my PCB design-rule check?
- No. Use both. EDA DRC checks the layout against electrical and spacing rules before export, while a Gerber viewer checks the exported manufacturing files for missing layers, mirroring, alignment, and rendering problems.
- Why do drill holes look shifted when the PCB editor looked correct?
- Shifted holes usually mean the Gerber and Excellon files were exported with different origins, units, or coordinate formats. Regenerate both outputs from the same CAM setup and verify them together.
- Should I inspect individual Gerber files or the ZIP?
- Inspect the final ZIP you plan to upload. Opening only individual files can miss missing layers, stale files, or drill files that were not included in the archive.
- What should I do if the viewer and fab DFM report disagree?
- Treat the fab report as process-specific and ask the manufacturer for clarification. A viewer shows the image data, but the fab's CAM tools evaluate the files against its equipment, stackup, and capability rules.