Back drilling removes the unused portion of a plated through hole after plating, so the via stops behaving like a stub. Everyone agrees on the principle. The argument starts when someone asks how short the remaining stub must be, because the answer is a frequency, not a length, and because the process that makes it short also makes the hole weaker and the depth uncertain.
1. Why a stub matters
A plated through hole that connects layer 1 to layer 4 still continues to layer 12 if the board has 12 layers. The unused length is a stub: an open-circuited transmission line hanging off the signal path. At low frequency it is invisible. As the wavelength approaches four times the stub length, the stub resonates and reflects, and the channel response shows a notch that no equalizer can recover cleanly.
The first resonance is roughly where a quarter wavelength equals the stub length in the dielectric. On an FR-4-class laminate with an effective dielectric constant around 4, a 1.5 mm stub resonates near 25 GHz. On a 2.5 mm stub it is closer to 15 GHz. At 25 Gbps NRZ, the signal content that matters extends past 12 GHz, so a 2.5 mm stub is already eating margin. At 56 Gbps PAM4 the same stub is a design error.
2. The length is not the depth on the drawing
Back drill depth is programmed, but the remaining stub is what survives. Three things decide it:
| Variable | Effect on remaining stub |
|---|---|
| Drill depth control | Depth repeatability of the machine, typically plus/minus 0.05 mm on a controlled process |
| Board thickness variation | Thickness varies across a panel and between panels; the drill references the surface, so the stub varies with it |
| Drill registration to the original hole | Off-center back drilling leaves a crescent of copper and a longer effective stub on one side |
| Dielectric constant at the target frequency | Decides what length is acceptable, and is not a single number |
This is why a specification written as "back drill to 0.25 mm stub" is not enough. What is needed is the acceptable stub range, the measurement method, and the sample plan. The fabricator controls depth; only the design controls whether the resulting resonance is inside the band of interest.
3. Choosing the target
Work backwards from the highest frequency that carries energy. Take the channel's Nyquist frequency, add margin for the transition band, and require the stub's first resonance to sit above it with some headroom. As a working rule we use a resonance at least 1.5 times the highest meaningful frequency.
That produces targets like 0.25 mm for 25 Gbps channels and 0.15 to 0.20 mm for 56 Gbps PAM4, on typical high-speed laminates. On very thick backplanes, where the drill cannot reach that deep without breaking through, the design answer is not a longer stub: it is a different via structure, a buried via, or a change in which layers the signal uses.
4. What back drilling does to the hole
It removes copper, and the copper it removes was doing mechanical work. Three consequences:
Barrel strength. The remaining barrel is shorter and the hole is now a blind structure from the back. Thermal cycling puts stress at the transition where the back drill stops. The depth has to leave enough barrel for the plating to remain continuous and for the annular ring on the last connected layer to survive.
Breakout risk. If the back drill goes too deep it can cut into the last signal layer's pad or into the plane below. The safe depth is set by the distance from the target layer to the next copper feature, not by the stub target alone. When those two conflict, the stack-up changes.
Contamination and solder wick. A back-drilled hole is open at one end. During assembly, flux and solder can wick into it. On press-fit connectors and on boards that go through wave solder, this has to be considered. Some designs call for the back-drilled end to be plugged, which adds a step and can reintroduce capacitance.
5. Measuring the result
There are three ways to know what you got, and they answer different questions.
Cross section. Destructive, definitive for a sample, and the only way to see the actual remaining stub and the plating condition at the transition. Take it through the worst-case via on the panel, in the region with the greatest thickness variation.
TDR on a via test structure. Non-destructive, shows the impedance profile along the via, and the stub shows as a dip and a reflection. Good for process monitoring per lot.
Channel measurement. The real answer, but it measures the whole channel, so it cannot separate stub from connector and package.
We report the cross-section result with the measurement location, and the TDR profile where the customer asks for it. A certificate that states "back drilled" without a number is not a result.
6. When not to back drill
Back drilling adds cost, adds a drill operation, and adds a failure mode. On boards where the highest meaningful frequency is below roughly 5 GHz, the stub is not the limiting factor and the money is better spent on the stack-up. On very high layer counts with signals that only use the top few layers, a buried via or a sequential lamination can solve the problem structurally instead of mechanically.
And on thin boards, the stub may already be short enough. A 1.6 mm board with signals on layers 1 to 3 has a stub under 1 mm; the resonance is far above the band and back drilling buys nothing.
7. Specifying it
On the fabrication drawing: which vias are back drilled, the acceptable remaining stub with a measurement method, the depth reference, the sample plan per lot, and the minimum barrel remaining at the transition. Add the stack-up with layer thicknesses, because the stub calculation depends on them and the fabricator cannot check the target without them.
The failures we see are all specification failures: a stub target that ignores breakout, a depth that assumes one board thickness on a panel that varies, and a first article that passes because it was sectioned in the thin part of the panel.
Send the stack-up and the channel target frequency and we will tell you what stub length is achievable on that build, and where the depth limit sits.
Related reading
- RF PCB DFM Checklist Before You Release the Gerber
- Lot-to-Lot Insertion Loss Variation on RF PCBs
- Cavity PCB Manufacturing: Depth, Flatness and Lid Interfaces
- Back Drilling Cost on High-Speed Backplanes
- RF Laminate Dk Drift with Temperature and Humidity
Need a DFM check or a stack-up review on your files? Write to pcba@superb-tech.com or WhatsApp +86 133 9608 1443.