PCB DFM Checklist: 10 Things to Check Before You Export Gerbers
Most fabrication holds come from a short list of layout issues. Run these ten checks before you export your files and your board is far more likely to pass review the first time.
A design rule check in your CAD tool tells you the layout obeys the rules you typed in. It does not tell you whether a factory can build the board at a sensible yield. That is what design for manufacturing (DFM) review is for, and most of what it catches comes from a short list of repeat offenders.
The values below are typical for standard-process rigid boards. They are a starting point. Tighter features are often possible, but they narrow your choice of process and raise the price, so confirm the limits for your build before relying on them.
1. Trace width and spacing
Check the narrowest trace and the smallest gap on every copper layer.
| Copper weight | Comfortable minimum width / spacing |
|---|---|
| 1 oz | 0.15 mm (6 mil) |
| 2 oz | 0.20 mm (8 mil) |
Thicker copper needs wider gaps because the etch undercuts the trace. If only one small area needs fine features, such as the breakout under a BGA, keep the rest of the board relaxed.
2. Drill sizes and annular rings
The annular ring is the copper left around a drilled hole. Drills wander slightly, so a ring that looks fine on screen can break out on the real board.
- Finished via hole: 0.3 mm or larger is a safe default
- Annular ring: at least 0.15 mm per side, so a 0.3 mm via gets a 0.6 mm pad
- Keep the number of distinct drill sizes low. Ten sizes that differ by 0.05 mm add tool changes and no value
3. Copper to board edge
Copper that runs to the edge can be exposed or torn when the board is routed out.
- Routed edges: keep copper at least 0.3 mm back
- V-scored edges: keep copper at least 0.5 mm back, since the score cuts into the board at an angle
This applies to planes as well as traces. Pull power and ground pours back from the outline.
4. Hole to copper clearance on inner layers
On multilayer boards, a plated hole passes through every layer. Any inner-layer copper that is not meant to connect needs clearance from the hole wall. Allow 0.25 mm or more. This is the check most often missed, because the problem is hidden inside the stack.
5. Solder mask between pads
The thin strip of mask between two adjacent pads is called a dam. If it is too thin, it flakes off and solder bridges the pads.
- Mask opening: 0.05 mm larger than the pad on each side
- Mask dam: 0.1 mm or wider
On fine-pitch parts where a dam will not fit, define one mask opening across the whole row on purpose. Do not leave it to chance.
6. Silkscreen
- Line width 0.15 mm or more, text height 1.0 mm or more
- No silkscreen on pads. Fabricators clip it away, and the clipped text may be unreadable
- Mark pin 1 and polarity so they stay visible after the parts are placed
7. Fiducials
Pick-and-place machines find the board using fiducial marks. Without them, placement accuracy suffers.
- Three global fiducials near the corners, placed asymmetrically so the board cannot be loaded rotated
- A 1 mm bare copper dot inside a 2 mm solder mask opening, with no other copper or silkscreen in that opening
- A local pair of fiducials next to any fine-pitch BGA or QFN
8. Component clearance to the edge
Conveyors grip the board by its edges. Keep parts at least 3 to 5 mm from the two long edges, or add break-away rails. The board flexes when a panel is separated, and that can crack ceramic capacitors. Keep them away from V-score lines and orient them parallel to the line.
9. Thermal relief and copper balance
A small pad tied directly to a large plane loses heat faster than the iron or oven can supply it. The result is a cold joint, or a small part standing up on one end.
- Use thermal relief spokes on through-hole pins and on small surface-mount pads that connect to planes
- Keep the two pads of a small passive thermally similar: same trace width in, same copper area
- Balance copper across the stack. A board with a solid plane on one side and almost nothing on the other tends to bow
10. Vias in pads
An open via inside a pad wicks solder away from the joint. Either move the via out and connect it with a short trace, or specify filled and capped vias. Filled vias are a different process with a different price, so call them out on purpose.
Before you export
- The board outline is a single closed shape on its own layer
- Every layer comes from the same revision
- Paste layers are included if the board will be assembled
- Board thickness, copper weight, and surface finish are written down somewhere other than your memory
What review catches, and what it does not
A fabricator's engineering review will flag features that cannot be built: spacing below the process limit, missing outlines, broken annular rings. It will not question whether your design is correct. A footprint with the wrong pin order passes review and still does not work.
Once your layout passes these checks, the next step is the file package. See what to send for a PCBA quote for the Gerber, BOM, and placement file requirements.
Related articles
PCB Assembly
Each assembly test finds a different kind of defect, and none of them finds everything. Here is what each one catches, what it misses, and how to pick a combination that fits your board and volume.
PCB Manufacturing
The surface finish protects the copper pads until the board is soldered. Here is how the three most common finishes differ in flatness, cost, and compliance, and which one fits your design.
Ordering Guide
A PCBA quote is only as fast as the files behind it. Here is what each file is for, what goes inside it, and the mistakes that most often send a quote back with questions.
