A DFM Checklist to Run Before You Send Gerber Files
Ten minutes of checking before upload removes most engineering queries. The data package contents, the geometric checks and the stack-up items that trigger an EQ.
Check five things before you upload: that every layer is present, that the drill file units match the Gerber units, that the board outline is on a mechanical layer, that the smallest annular ring is above the process limit, and that the smallest clearance is above the process limit. Those five catch the large majority of engineering queries.
An engineering query is not a rejection. It is a question that has to be answered before the board is released, and every query adds time to the lead clock. The checklist below is what we run on incoming data, in the same order.
01Data package contents
A complete package lets the board be built without assumptions. Missing layers are the single most common cause of a delayed quote.
- One Gerber file per copper layer, named so the layer order is unambiguous
- Solder mask top and bottom
- Legend or silkscreen top and bottom
- Paste layers top and bottom, if the board will be assembled
- Drill file in Excellon format, with plated and non-plated holes separate
- Board outline on a mechanical layer, closed contour, with dimensions
- Stack-up drawing for any board with four or more layers
- Impedance requirements with target, tolerance and reference layer
- A README stating units, layer count, board thickness and copper weight
02Geometric checks
These are the numbers that decide whether the board can be made at all, and they are all visible in your CAD tool before export.
| Units | Gerber and drill must use the same unit. A 2.5 imperial drill file against a metric Gerber shifts every hole |
|---|---|
| Annular ring | Minimum half the difference between pad diameter and drill diameter. Below the process limit the drill breaks out of the pad |
| Clearance | Trace to trace and trace to pad. Check the tightest point in the board, not the typical value |
| Drill to copper | Distance from a drilled hole edge to the nearest unrelated copper. Too small causes a short after plating |
| Board outline | Must be a closed contour on a mechanical layer, with the routed dimension matching the copper keepout |
| Solder mask sliver | Mask between two adjacent pads. Below the minimum width the mask bridge will not survive processing |
03Stack-up and electrical checks
For multilayer boards, confirm that the layer order in your stack-up matches the Gerber file names, that the dielectric thicknesses add up to the total board thickness, and that the copper weights are stated as finished rather than starting weight.
If the board has controlled impedance, state the target, the tolerance, the layer and the reference plane for every controlled net. A stack-up without those four items cannot be verified, and the factory will either query it or build to its own standard structure.
04What triggers an engineering query
These are the items that most often stop a board from being released, in rough order of frequency.
- Missing or ambiguous layer, especially a missing solder mask or drill file
- Annular ring below the process limit for the specified drill size
- Copper clearance below the limit for the specified copper weight
- Board outline that does not close, or dimensions that conflict with the copper
- Impedance requirement stated without a reference layer or stack-up
- Drill file units that do not match the Gerber units
- Solder mask bridges narrower than the process minimum between fine-pitch pads
- Copper to board edge distance smaller than the routing tolerance allows
Key takeaway
Export every layer, match the units between Gerber and drill, close the board outline, and check annular ring and clearance against the process limit before you upload. It removes most engineering queries and shortens the quote.
Products discussed in this article
Continue reading
Ready to start your project?
Send your Gerber files for a quote. Simple boards are quoted within 1 hour, complex builds within 24 hours.