Gerber Viewer: How to Check Your Files Before You Order

The short answer

A Gerber viewer opens the exact files your fabricator will read and shows each layer as plotted. The free options are KiCad’s own Gerber Viewer, the open-source desktop program gerbv, and browser viewers that run locally or on the fab’s upload page. Whichever you use, load the files you are about to upload, not the board in your editor. The point is to catch export mistakes, and those only exist in the exported files.

Which viewer to use

KiCad Gerber Viewer. It installs with KiCad and opens from the project manager. It loads Gerber layers, Excellon drill files, and the Gerber job file together, and lets you toggle layers and measure. If you already designed in KiCad, this is the lowest-friction choice because it uses the same install and nothing is uploaded anywhere.

gerbv. A small open-source viewer common on Linux and available for other platforms. It overlays layers with transparency and is useful when you are checking files produced by a tool other than KiCad.

Browser viewers. Several fabs render your upload as soon as you drop in the zip, and independent browser viewers exist as well. These are convenient and good for a second opinion, but a fab’s preview shows how that fab interpreted the files, which is useful in its own right: it is the interpretation that will be manufactured. If the files are confidential, prefer a viewer that runs locally.

Using two viewers is a cheap habit. If both draw the same board, the files are unambiguous. If they disagree, a layer is probably mis-identified or an aperture is unusual, and a human at the fab may have to guess.

The six-point check

Load all copper, mask, silk, edge, and drill files, then look for the following.

1. File count matches the layer count. A two-layer board needs front and back copper, front and back mask, the board outline, and drill data, plus silkscreen if you want it. Missing the outline or drill file is the most common reason for a fab to stop and email you.
2. The outline is one closed loop. Show only the edge layer. A gap of even a fraction of a millimetre can leave the fab guessing where to route the board. Slots and cutouts should be closed shapes too.
3. Drill hits sit centred on pads. Overlay the drill file on copper. A hole that lands off-centre, or plated holes missing on a connector footprint, means the drill export used a different origin from the Gerbers. Use the same origin for both.
4. Mask openings line up with pads. Mask is usually plotted as the opening, so pads appear where the mask is open. Pads that are covered, or openings far larger than the pad, point to a wrong mask setting.
5. Silkscreen stays off exposed copper. Text over pads is trimmed or ignored by many fabs, but it makes the board harder to read and can hide polarity marks. Move it before ordering.
6. Bottom layers read correctly. Viewers show the bottom side as if you flipped the board. Text on the bottom silkscreen should read normally in that view, not mirrored.

For a board with a ground pour, also look at the copper layer with zones visible. Stale or unfilled zones are a design-side problem (refill zones before plotting) that shows up here as missing copper.

What a viewer cannot tell you

Seeing a clean render does not mean the board works. A viewer checks geometry against your intent; it does not check the schematic, part values, pin assignments, or whether the nets in the layout match the circuit. It also does not apply your fab’s minimum trace, spacing, or drill limits. Those come from running the design-rule check in your editor against the fab’s published capabilities, which is covered in the DFM checklist.

If you want that whole sequence run for you, the MakeIRL preflight gate runs ERC, DRC, schematic parity, BOM completeness, and export integrity on the KiCad project and returns BLOCKED, REVIEW, or READY. It is an automated check, not a human review, and it does not claim the board will function. A sample report is at /preflight/sample.

A quick routine you can repeat

1. Refill zones, run DRC, and fix errors in the editor.
2. Plot Gerbers and drill files to a clean folder (see exporting Gerbers from KiCad for JLCPCB).
3. Open the folder in a viewer and run the six checks above.
4. Zip only the files in that folder and upload.
5. Look at the fab’s own preview and compare it with your viewer’s render before paying.

New to the formats themselves? What is a Gerber file explains what each file contains and why drill data is separate.