Contact Us
  • Home
  • BLOG
  • RF PCB DFM Checklist Before You Release the Gerber

RF PCB DFM Checklist Before You Release the Gerber

Most RF boards that fail do not fail in simulation. They fail at the point where a design rule that was fine at DC meets a fabrication process that has tolerances of its own. A DFM review is not a checklist for its own sake; it is the cheapest place to catch the twenty or so decisions that cost money after the panel is pressed.

These are the checks we run on an RF or mixed-signal board before quoting, grouped by what they protect.

1. Stack-up

CheckWhy it matters
Every controlled line has a solid reference plane directly below or aboveImpedance is set by the reference, not by the trace width alone
No plane split crosses a controlled lineA split forces the return current around the gap and changes impedance locally
Dielectric thickness is specified per layer, not by total board thicknessLamination controls each layer; total thickness hides the one that matters
Material choice matches the frequency and the loss budgetFR-4 is fine at 3 GHz and wrong at 30 GHz; the substrate is a cost decision made too late
Prepreg and core part numbers are namedWithout them, "equivalent" substitutions appear at the fabricator
Symmetry around the center lineAsymmetric builds warp, and warpage breaks assembly, not fabrication

2. Copper and routing

Minimum line width and spacing against the copper thickness being ordered. A 0.1 mm line on 1 oz copper is a different process from 0.1 mm on half-ounce, and both are different from 0.075 mm. Quoting a design at a line width the copper weight cannot support is the most common early failure.

Trace width compensation for the target impedance, given the laminate. Do not carry an FR-4 width onto a PTFE stack because the number looked the same. The Dk difference is large enough to move a 50 ohm line by 15 percent.

Ground pour spacing and via stitching along the RF path. A pour that is stitched at 5 mm intervals is not a shield at 10 GHz; the spacing has to be a fraction of the wavelength in the dielectric.

Thermal relief on pads that need to solder, solid connection on pads that need to conduct heat or RF. The two requirements conflict and the choice has to be per pad, not global.

3. Vias

Via aspect ratio against the finished board thickness. Above roughly 8:1 the plating uniformity becomes the limiting factor, and above 10:1 the process is a specialist one. If the design needs 12:1, that is a conversation to have before the layout is finished.

Via in pad: filled or not, capped or not, and which IPC-4761 type. An unfilled via in a thermal pad wicks solder and leaves a void that shows up as a hot spot.

Back drilling: which vias, what stub, and whether the depth conflicts with the plane below. A stub target that cuts into the next layer is a scrap lot, not a tolerance issue.

Via annular ring on the finished hole, on the worst layer, measured after plating. On high layer counts the inner-layer ring is the one that fails, not the outer.

4. Pads and footprints

Footprint geometry against the component datasheet, including the recommended land pattern and the thermal pad dimensions. A thermal pad drawn 0.1 mm small prints paste onto the mask and produces a tilted part.

Solder mask clearance around pads. Too little and the mask lifts; too much and solder bridges between fine-pitch leads.

Paste aperture ratio for the finest pitch on the board. Below about 0.66 area ratio the paste release becomes unreliable, and that is a stencil decision that has to be made at design time, not at assembly.

Component orientation and courtyard for the pick-and-place. A part rotated 90 degrees in the CAD data is a reflow defect at 2 a.m. on the line.

5. Solder mask, finish and legend

Finish choice against the assembly and the RF requirement. ENIG is flat and good for fine pitch; it is also lossy at mmWave if the nickel is thick. Immersion silver and bare copper have their own constraints. The finish is part of the electrical design on high-frequency boards, not just a corrosion coating.

Mask dam width between pads. On 0.4 mm pitch, the dam has to be narrow enough to fit and wide enough to survive, and that is a fabrication limit, not a preference.

Legend that does not print over pads or into via holes. Legend ink in a via is a plating and assembly problem.

6. Panel and mechanical

Board size against the panel. A board that fits six per panel is priced differently from one that fits four, and the difference is often larger than the material upgrade being debated.

Break-away and route separation with enough material left to survive assembly. V-groove depth, tab width, and whether the board is handled by the edge or by the surface.

Hole-to-board-edge distance. Copper closer than 0.3 mm to the rout line is a plating and handling risk, and on an RF board the edge is often where the ground pour is thinnest.

Warpage allowance. A 1.6 mm board with a large copper imbalance will bow, and the assembly house will reject it before the customer sees it.

7. Documentation

Gerber layers with a clear naming convention, drill file with plated and non-plated separated, and a fabrication drawing that states the stack-up, the impedance targets, the finish, the via protection type, the tolerance on the mechanical outline and the acceptance standard.

If the drawing says "IPC Class 2" and the assembly drawing says "Class 3", the board will be built to whichever the fabricator reads first.

8. The five that actually cost money

In our experience the expensive ones are not exotic. A stack-up that cannot hold the impedance the layout assumed. A via in pad with no fill type specified. A line width quoted below what the copper weight supports. A panel that fits four boards instead of six because 3 mm was added to the outline. And a finish chosen for cost that has to be changed after the first RF measurement.

All five are visible in a DFM review that takes an hour. None of them are recoverable after lamination.

Send the Gerber and the stack-up and we will return the DFM notes with the process limits that apply to that build, before you release the order.

Related reading

Need a DFM check or a stack-up review on your files? Write to pcba@superb-tech.com or WhatsApp +86 133 9608 1443.