How to check your Gerbers before you order
A step-by-step checklist for spotting the common Gerber export mistakes in any online Gerber viewer, before a manufacturer builds boards you can't use.
Last reviewed
This checklist works in any of the ranked viewers that open Gerber and drill files. Do it on the exact ZIP you're about to upload, not on the files you think you exported. Most bad boards come from a small number of export mistakes, and almost all of them are visible in a viewer in a few minutes.
Before you start
- Open the ZIP itself. Unzip a copy and look at the file list. Old exports from earlier revisions sitting in the same folder are a classic way to send the wrong board.
- Know your board. Have the layer count, the board size and roughly what it should look like in mind before you open it.
The checklist
1. Count the files
Compare the file list with what a complete package holds: copper for every layer, mask, silkscreen, outline and drill. A 4-layer board needs four copper files. Missing a layer is the commonest mistake, and the viewer will happily show a board without it.
2. Check every file landed on the right layer
Many viewers guess each file's layer from its name. Look at the layer list: is the top copper really top copper, and is the outline shown as the outline and not as a copper layer? Gerber X2 files carry their layer in the file, which avoids most of this.
3. Check the outline is one closed shape
Turn off everything but the outline. You should see one continuous loop around the board, plus closed shapes for any internal cutouts. Gaps, overlapping duplicates, or lines that stop just short of each other confuse the fab's routing. Text or dimension lines on the outline layer will be read as cuts.
4. Check the holes line up with the pads
Turn on the drill layer over the copper. Every via and through-hole pad should have a hole centred in it. If all the holes are shifted by the same amount, the drill file uses a different origin from the Gerbers. If the hole pattern is the right shape but much bigger or smaller, the units or the number format differ. Re-export both with the same origin and units.
5. Check plated and non-plated holes
Mounting holes that must not be plated should be in the non-plated (NPTH) file. Slots and oval holes should appear as slots, not as a single round hole.
6. Measure the board
Use the viewer's measuring tool on the outline. Does the width and height match your enclosure and what you'll enter on the order form? A board exported in the wrong unit is often off by a factor of 25.4.
7. Check copper pours are filled
Look at your ground planes and pours. If they show as outlines, or are missing, the zones weren't filled before export. In KiCad, refill zones (or tick the option to check zone fills before plotting) and export again.
8. Check the solder mask openings
View the mask layer over the copper. Every pad you'll solder needs an opening. Vias you wanted covered ("tented") should not have openings. Large missing areas usually mean the mask layer was exported from the wrong side or not at all.
9. Check the silkscreen
Text should be readable and not printed over pads. Bottom-side text looks mirrored when you view it from the top; that's correct. Text that reads normally from the top on the bottom layer will come out backwards.
10. Check paste, if you're ordering assembly or a stencil
Paste openings should sit on surface-mount pads only, with none on through-hole pads or fiducials you didn't mean to paste.
11. Compare with the fab's own preview
After uploading, look at the manufacturer's preview too. If it differs from what your viewer showed (a missing layer, a different outline), stop and find out why before paying.
The mistakes this catches
| What you see in the viewer | Likely cause | Fix |
|---|---|---|
| Holes offset from pads | Drill file and Gerbers use different origins | Export both with the same origin setting |
| Holes the wrong size or scattered | Drill units or number format don't match | Export drill files in mm with decimal format |
| A copper layer is missing | Layer not selected when plotting | Re-plot with every copper layer ticked |
| Pours show as outlines or are absent | Zones not filled before export | Refill zones, then plot |
| Outline has gaps or extra lines | Open shape, or drawings on the outline layer | Close the outline; move notes to another layer |
| Board size is wildly off | Wrong unit in the export | Re-export in mm |
Exported from KiCad?
The KiCad settings that prevent most of these are in Exporting Gerbers from KiCad. And if you have the KiCad project, opening it alongside the Gerbers shows you what the copper was meant to be: see Gerber files versus design source files.