DFM: 12 rules that save you costly PCB manufacturing mistakes

DFM (Design for Manufacturability) means designing a board so that it can be manufactured, assembled and tested without special measures, exceptions or back-and-forth with the manufacturer. A board that looks perfect on screen can cause a lower yield in the factory, assembly defects or even non-functional boards. Below are twelve rules we check on every board before it goes into production.

1. Design to the manufacturer's capabilities, not to the minimum

Every manufacturer publishes its technology capabilities: minimum trace width, minimum clearance, smallest hole, minimum annular ring. Typical values for standard technology:

The rule: in your layout keep at least a 20 per cent safety margin above the minimum. A board with 0.2 mm traces and 0.2 mm clearances will have a better yield and a lower price, and will suit more manufacturers than a board right at the 0.1 mm limit.

2. Sufficient annular rings

The annular ring is the copper around a hole after drilling. The drill has a tolerance of about 0.05 to 0.1 mm, so an annular ring that is too small means breakout and a weak or broken connection. For vias use a pad at least 0.25 mm larger than the hole (e.g. a 0.3 mm hole with a 0.6 mm pad); for THT components a pad at least 0.5 mm larger than the hole. For connectors subject to high forces, increase the ring further.

3. Copper clearance to edges and cut-outs

Edge routing has a tolerance of about 0.1 to 0.2 mm. Copper that reaches the edge can peel off or short to the enclosure. Keep at least 0.3 mm (preferably 0.5 mm) between copper and the edge, and for V-cut scoring at least 0.4 mm from the centre of the score. Copper pours (GND) should have a clearance to the outline set in the design rules.

4. Solder mask between pads

With fine-pitch packages (QFN, QFP with 0.5 mm pitch) it is important that a solder mask dam at least 0.1 mm wide remains between the pads. Check the mask expansion in your footprints: if it is too large, neighbouring openings merge and solder bridges form more easily. Where the dam cannot be kept, opt for a common opening – but that requires a more precise stencil.

5. Silkscreen that does not get in the way

The silkscreen is for people, not machines, yet it can still cause problems:

• text should be at least 1 mm high with a line width of 0.15 mm, otherwise it is illegible;
• silkscreen must not cross pads, as solder will not wet there;
• component designators should sit outside the footprint and be oriented consistently (in two directions, not four);
• the polarity of diodes and capacitors and pin 1 of ICs must be marked unambiguously;
• add the name, revision and date to the board, so that a year from now you know what you are holding.

6. Fiducial marks for assembly

Fiducials are round copper pads (1 mm diameter) with a 3 mm mask-free area that the pick-and-place machine uses for alignment. The rules:

• at least two, preferably three per board, in the corners and placed asymmetrically so the orientation cannot be confused;
• at least 5 mm from the edge of the board and the panel;
• add local fiducials next to fine-pitch BGAs;
• on a panel, add fiducials to the frame as well.

Without fiducials, placing 0402 and QFN components is not reliable, because the tolerances of the board outline are larger than the placement tolerance.

7. Thermal reliefs on pads in copper pours

A pad connected directly to a large copper area conducts heat away so fast that the solder does not melt properly; the result is cold joints and tilted components (tombstoning). Use thermal reliefs with four spokes 0.3 to 0.5 mm wide for THT components and passive SMT components. The exception is power pads (e.g. the exposed pad under a QFN or regulators), where the thermal connection is deliberately solid; there, thermal vias and a slightly thicker paste layer help.

8. Even copper distribution

An uneven amount of copper on the layers (one side full, the other almost empty) causes the board to warp during manufacturing and reflow. Add copper pours to sparsely populated layers too, and consider hatched fills for very large areas. On multilayer boards the stackup should be symmetrical.

9. Vias in pads and untented vias

A via inside an SMT pad wicks away the solder and creates a poor joint, unless the via is filled and capped (via-in-pad, plugged and capped), which is a more expensive technology. On standard boards move vias at least 0.3 mm away from the pads and, where possible, cover them with solder mask (tented) to prevent shorts during testing and corrosion. Leave open the vias that will serve as test points.

10. Test points and test access

Plan already in the layout how you will test the board:

• test points (pads of 1 mm diameter or more) on all power rails, reset, communication buses and key signals;
• all test points on one side, at least 2.54 mm apart if you expect a bed-of-nails test fixture;
• a programming connector or probe pads (e.g. Tag-Connect) for loading firmware without a connector;
• consider keeping JTAG/SWD access in the series product as well – just covered and unpopulated.

11. Panelisation for assembly

Boards smaller than about 50 × 50 mm, or boards with irregular shapes, are assembled in a panel so that the machine can process them. The rules:

• the panel should have a frame at least 5 mm wide with two fiducials and tooling holes;
• choose V-cut for rectangular boards (cheaper, no residue) or mouse bites and routed slots for rounded shapes;
• with V-cut, keep components at least 1 mm from the score; with mouse bites at least 2 mm;
• components that overhang the board edge (connectors) require routing and extra space;
• choose panel dimensions supported by your assembly provider (typically up to 250 × 350 mm).

12. Complete and consistent documentation

Most delays are caused by a mismatch between the Gerbers, the BOM and the placement (pick-and-place) file:

• the BOM should contain the designator (R1, C3), value, package, manufacturer and manufacturer part number, ideally with an alternative;
• the placement file should give coordinates in millimetres relative to the same origin as the Gerbers, with rotation according to the standard (an agreed pin 1 position);
• mark the components that are not to be placed (DNP);
• include an assembly drawing with marked polarity and special instructions (e.g. connector height, screw torques);
• define the revision; the same revision means the same files.

Quick DFM checklist

• Widths and clearances with a margin above the manufacturer's minimum
• Via annular rings of at least 0.15 mm, THT pads at least 0.5 mm wider than the hole
• Copper at least 0.3 mm from the edge
• Mask between the pads of fine-pitch packages
• Silkscreen not overlapping pads, clear polarity
• Three fiducials, asymmetric
• Thermal reliefs in pours, solid connection on power pads
• Even copper, symmetrical stackup
• Vias outside the pads, tented
• Test points on one side
• Panel with a frame, fiducials and suitable clearances
• BOM, placement file and Gerbers from the same revision

Need help?

A DFM review is part of every project we take into production at Selektronik, because a fix in the layout is always cheaper than a fix on a hundred boards. If your board is ready, upload the files to our PCB configurator and send an inquiry. If you want an independent DFM review before manufacturing, or help with panelisation and assembly documentation, have a look at our component assembly services.