How to check Gerber files before ordering a PCB
The Gerber files, not the design in your EDA tool, are what the manufacturer builds. A setting left unchecked in the fabrication output, a missing drill file or an outline on the wrong layer can turn into a batch of unusable boards. Reviewing the exported files takes a few minutes and catches most of these problems before they cost money.
1. Confirm that every layer is present
A two-layer board normally needs top and bottom copper, top and bottom solder mask, top and bottom silkscreen, the board outline and at least one Excellon drill file. Four-layer and six-layer boards add the inner copper layers. Load the archive in a Gerber viewer and compare the layer list against your stackup. A layer that is missing from the list was either not exported or has a file name the viewer does not recognise.
2. Check alignment between layers
All layers must share the same origin. Show the copper, solder mask and drill layers together and zoom into a few pads in different corners of the board: mask openings should be centred on the pads and drill hits should fall in the middle of the plated holes. A constant offset usually means that one file was exported with a different origin or with an auxiliary origin enabled.
3. Verify the board outline
The outline must be a single closed contour, with internal cut-outs drawn on the same layer. Check that no copper or silkscreen crosses it, that mounting holes are on the drill layer rather than drawn as outline circles if your manufacturer requires that, and that the overall dimensions match the mechanical drawing.
4. Review drills and annular rings
Confirm that plated and non-plated holes are in the correct file, that via drill sizes match what you specified, and that the copper ring left around each hole is above the manufacturer's minimum. Unusually large or small drill diameters are often the result of a unit mismatch between metric and imperial settings.
5. Inspect solder mask and paste
Every pad that will be soldered needs a mask opening, and fine-pitch parts need the slivers of mask between pads that your manufacturer can actually produce. Look for vias that should be tented but appear open, and for large copper pours that were exported without mask relief.
6. Read the silkscreen
Designators should be legible, not placed over pads and not cut by the outline. Bottom silkscreen should read mirrored when viewed from the top, which is correct. Check the text height against the manufacturer's minimum so that labels do not blur.
7. Keep a reference of what you ordered
Exporting a true-scale PDF of the top view, bottom view and each layer gives you a record of the exact files that went to fabrication and a printable 1:1 reference for placing components by hand. PCB Tools generates this vector PDF directly from the Gerber archive.
For the meaning of each file name in the archive, see Gerber file extensions explained.