A PCB order is only as clear as the manufacturing package you upload. Your EDA tool may have a clean board view, a passing design-rule check, and a tidy project tree, but the fab builds from exported Gerber and drill data. A missing outline, shifted drill file, or wrong bottom-layer orientation can survive until the upload step if you do not inspect the actual files.
Use this checklist after export and before payment. It is intentionally practical: confirm the complete layer set, confirm the drill data, confirm that file formats align, and then open the free Gerber viewer to look at the exact ZIP your manufacturer will receive.
If you are still deciding what belongs in the package, the complete PCB manufacturer file list separates bare-board fabrication files from assembly files such as the BOM and pick-and-place data.
Quick answer
Before ordering, check that your ZIP contains the required Gerber layers, Excellon drill files, a closed board outline, consistent units and origin, correct bottom-layer orientation, clean silkscreen, and fabrication notes. Then load the ZIP in a Gerber viewer and confirm every layer visually.
Pre-order Gerber checklist
- Complete layer set. A normal two-sided PCB needs top copper, bottom copper, top solder mask, bottom solder mask, top silkscreen if used, bottom silkscreen if used, and a board outline or edge-cuts layer. Paste layers are different from solder mask. Include top paste and bottom paste when ordering a stencil or assembly, but do not treat them as required for a bare PCB.
- Correct board outline. The outline should be present, closed, and on the expected mechanical or outline layer. It should define the true finished board size, including slots, internal cutouts, tabs, mouse bites, or unusual routing features. A rectangle drawn on silkscreen is not a manufacturing outline.
- Excellon drill files included. Copper pads show where holes should land, but they do not tell the drill machine what tool diameter to use. Include Excellon drill output for vias, through-hole pads, slots, and mounting holes. If your CAD tool exports plated through holes and non-plated holes separately, include both files and label them clearly.
- PTH and NPTH are distinguished. Plated holes receive barrel copper and connect layers. Non-plated holes are normally mechanical holes with no barrel plating. The difference affects both fabrication and electrical behavior, so mounting holes, tooling holes, and slots should be assigned deliberately.
- Units and coordinate format are consistent. Gerber and drill files must agree on units, origin, and coordinate precision. Common modern exports use metric or inch coordinates with formats such as 2:4, 2:5, or 4.6 depending on the tool. A Gerber file can look normal by itself while the drill file shifts if the format is interpreted differently.
- Bottom layers are oriented correctly. Most PCB fabs expect bottom layers in the same board coordinate system as viewed from the top, not manually mirrored a second time by the designer. If bottom copper or bottom silkscreen looks reversed relative to holes and the outline, review the export settings before ordering.
- Silkscreen clears pads and exposed copper. Component text and polarity marks should not print over solderable pads, test pads, castellations, or exposed copper. Many fabs clip silkscreen automatically, but relying on clipping can remove reference designators or leave unreadable marks.
- Manufacturing dimensions match your fab capability.Minimum trace width, copper spacing, drill size, solder mask sliver, copper-to-edge clearance, and annular ring should follow your chosen manufacturer capability table. Typical prototype services publish standard and advanced limits, but there is no universal number that applies to every board thickness, copper weight, and process.
- No missing apertures or unrendered draws. RS-274X and Gerber X2 files should contain embedded aperture definitions. If a viewer shows missing pads, broken pours, odd flashes, or empty files, regenerate the output and check whether old CAM settings or unsupported primitives are involved.
- Fabrication notes are included when needed. A simple two-layer board may only need order-form choices, but controlled requirements should be written down: material, finished thickness, copper weight, solder mask color, surface finish, impedance stackup, panelization instructions, via tenting, and any special tolerance.
- ZIP structure and file names are sensible. Put the current manufacturing outputs in one ZIP. Avoid nested project folders, old exports, screenshots, and unrelated CAD files. Use clear extensions or names such as top copper, bottom copper, top mask, outline, PTH drill, and NPTH drill so a CAM reviewer can identify the files quickly.
Checklist reference
| Checklist item | Why it matters | How to verify |
|---|---|---|
| Layer set | Missing copper, mask, silk, or outline changes the board. | Toggle each layer in the viewer and compare with the order. |
| Board outline | The fab needs the finished size and routed shape. | Check for one closed profile on the outline layer. |
| Drill files | Vias and through-hole pads require tool sizes and locations. | Overlay drill hits on copper pads and mounting holes. |
| PTH / NPTH split | Plating status changes electrical and mechanical behavior. | Inspect separate drill outputs or drill legend notes. |
| Units and origin | Mismatches shift layers, holes, or the board outline. | Confirm all files register at the same coordinate system. |
| Silkscreen clearance | Ink on exposed copper can be clipped or cause process issues. | Overlay silkscreen with mask and copper openings. |
| Fab capability | Too-small geometry can increase cost or fail DFM review. | Compare design rules with the manufacturer's published limits. |
| ZIP contents | Stale or unclear files slow CAM review and risk wrong builds. | Open the final ZIP, not just the output folder. |
Common mistakes to avoid
- Exporting Gerbers but forgetting Excellon drill output. Drill files are not optional for boards with vias, through-hole components, slots, or mounting holes.
- Sending an old ZIP after making a final board change. Regenerate into a clean folder and archive only the current outputs.
- Assuming the order form replaces fabrication notes. The order form is useful, but controlled requirements should also be present in drawings or notes when they affect acceptance.
- Manually mirroring bottom Gerbers because the bottom layer looks backward in the PCB editor. Export tools already know which side is bottom; manual mirroring can double-mirror the manufacturing data.
- Treating silkscreen as documentation only. Silkscreen is a physical ink layer and must clear pads, exposed copper, board edges, and small solder mask openings.
Check the final ZIP in the viewer
The final step is to inspect the exact archive you plan to upload. Use the Gerber viewer to load the ZIP, toggle every visible layer, and check registration between copper, solder mask, silkscreen, board outline, and drills. Do not rely only on the PCB editor display because export settings can omit layers, change coordinate origin, or leave old files in the output folder.
For a second pass, follow the more detailed visual workflow in how to check Gerber files for errors. That guide focuses on what export mistakes look like in a viewer and how to combine visual inspection with EDA DRC and the fab's DFM report.
FAQ
- Do I need to include paste layers when ordering a PCB?
- Include paste layers when you are ordering a stencil or asking for assembly. For bare board fabrication only, paste layers are usually not required because solder paste is not part of the board fabrication process.
- What should I do if my fab says the Gerber files are incomplete?
- Ask which layer or drill file is missing, then regenerate the package from your PCB editor into a clean output folder. Verify that copper, mask, silkscreen, outline, and Excellon drill files are all present before uploading the ZIP again.
- Does it matter whether Gerbers use metric or imperial units?
- Either metric or imperial can work, but the Gerber and drill files must use consistent units, coordinate format, and origin. A mismatch can shift holes or layers even when each individual file opens.
- Is a board outline file required?
- Yes. The manufacturer needs a clear board outline or route layer that defines the finished shape, size, slots, and cutouts. Without it, the CAM operator has to guess the profile or reject the upload.