PCB Back Drill: Why, When, and How to Specify It

Via stubs are invisible parasites in your signal path. They do nothing useful — they are the unused portion of a plated through-hole via that extends beyond the signal layer into empty board space. At low frequencies, stubs are harmless. At 5GHz and above, they become resonant structures that create insertion loss notches, degrading or destroying multi-gigabit signals.

Back drilling removes the stub. This guide covers when you need it, how it works, and how to specify it.

The Via Stub Problem

What Creates a Stub

When a signal transitions from Layer 1 to Layer 3 through a plated through-hole via in a 16-layer board, the via extends from Layer 1 to Layer 16 — but only the portion from Layer 1 to Layer 3 carries signal. The remaining portion (Layer 3 to Layer 16) is the stub.

L1  ───►  Via  ◄─── Signal enters here
L2        │
L3  ───►  Via  ◄─── Signal exits here
L4        │
L5        │
...       │     ◄─── This is the STUB
L14       │         (unused via length)
L15       │
L16  ─────┘

Why Stubs Cause Problems

A via stub behaves as a shorted transmission line. It has a resonant frequency where it presents very low impedance to the signal — effectively a short circuit at that frequency:

f_resonance ≈ c / (4 × L_stub × √Dk_eff)

Where:

• c = speed of light (3×10⁸ m/s)
• L_stub = stub length
• Dk_eff = effective dielectric constant (~3.8-4.2 for FR4)

Stub Resonance Table

Rule of thumb: Signal degradation begins at approximately 1/3 of the stub resonance frequency. A 100mil stub resonates at 7.5GHz but begins degrading signals around 2.5GHz.

Insertion Loss Impact

For a 25Gbps NRZ signal (Nyquist frequency 12.5GHz) with a 60mil via stub:

At 12.5GHz (the Nyquist frequency of 25Gbps NRZ), a 60mil stub costs 7.9 dB of insertion loss. This is catastrophic for signal integrity — most SerDes receivers need the channel loss below 20-25 dB total.

How Back Drilling Works

The Process

Back drilling (also called controlled-depth drilling or stub removal) is a second drilling operation performed after the board is fully fabricated:

1. Standard fabrication — Board is manufactured normally with plated through-hole vias
2. Registration — Board is mounted on the drill machine with X-ray alignment to locate via positions
3. Controlled-depth drilling — A larger-diameter drill enters from the opposite side, removing the plated copper and stub portion
4. Depth verification — Cross-section or X-ray confirms residual stub length

Drill Parameters

Back Drill Diameter Selection

The back drill must be large enough to completely remove the plated copper on the via wall:

Engineer’s Note: The back drill hole must clear the plated barrel on all sides, accounting for drill registration tolerance (±2mil) and original via position tolerance (±2mil). Add at least 4mil per side to the plated hole diameter.

Ready to Build Your Next PCB?

From prototype to production — complex boards engineered right. HDI, RF, high-layer-count FR-4, and more.

Get Instant Quote →

When to Specify Back Drilling

Decision Matrix

Backplane-Specific Considerations

Server and networking backplanes are the primary application for back drilling:

• Board thickness: 100-250 mil (2.5-6.35mm)
• Layer count: 16-40+ layers
• Via stubs: often 100-200mil (50-80% of board thickness)
• Signal rates: 25G-112G per lane

Without back drilling, these stubs make multi-gigabit signaling physically impossible. Back drilling is a standard line item on every high-speed backplane BOM.

Design Rules for Back Drilling

Pad and Anti-Pad Sizing

The back drill hole is larger than the original via — ensure adequate anti-pad clearance on all layers that will be back-drilled:

Example: For a 12mil via with 24mil back drill:

• Standard anti-pad on connection layers: 24mil (12mil drill + 6mil annular ring per side)
• Back-drill anti-pad on all other layers: 40mil (24mil back drill + 8mil clearance per side)

Drill-to-Drill Spacing

Back drill holes need adequate spacing to prevent structural weakness:

Back Drill from Both Sides

Some designs require back drilling from both sides of the board — for example, when signals route on middle layers of a thick board:

Back drill from TOP side (removes stub above L8)
         ↓
L1   ────┐
L2       │  ← Back drilled from top
L3       │
L4       │
L5       │
L6       │
L7       │
L8   ────┤  ← Signal layer
L9       │
L10      │  ← Back drilled from bottom
L11      │
L12  ────┘
         ↑
Back drill from BOTTOM side (removes stub below L8)

Dual-side back drilling requires two registration setups and two drill passes — cost increases by approximately 30-50% over single-side back drilling.

Alternatives to Back Drilling

Back drilling is the most cost-effective solution for high-speed through-hole vias in boards >8 layers. Blind vias and HDI eliminate stubs entirely but at significantly higher cost.

When to Use Blind Vias Instead

• Stub residual from back drilling (5-10mil) is unacceptable (112G+ channels)
• Via count is low enough that blind via cost is manageable
• Board already requires HDI for other reasons (fine-pitch BGAs)

Verification and Quality Control

Depth Verification Methods

Acceptance Criteria

Specifying Back Drilling in Your Fab Drawing

Include the following in your fabrication notes:

BACK DRILL REQUIREMENTS:
- All vias marked "BD" in drill file shall be back drilled
- Back drill from [TOP/BOTTOM/BOTH] side(s)
- Back drill target: remove stub to within 10 mil of [Layer X]
- Back drill diameter: [XX] mil
- Residual stub tolerance: +5/-0 mil from target layer
- Depth tolerance: ±4 mil
- Verification: cross-section on first article + X-ray on production

Provide a separate drill file or drill table for back drill locations. Clearly mark which vias require back drilling — not all vias need it (only those carrying high-speed signals).

Design Checklist for Back Drilling

• Identify all vias carrying signals >5GHz (or >10Gbps NRZ / >25Gbps PAM4)
• Calculate stub length for each critical via
• Verify stub resonance frequency vs. signal bandwidth
• Size anti-pads on all back-drilled layers (back drill diameter + 16mil)
• Verify back drill diameter clears plated barrel (including registration tolerance)
• Check drill-to-drill spacing (back drill + 10mil minimum)
• Determine single-side or dual-side back drilling
• Specify residual stub target in fab notes (5-10mil typical)
• Create separate back drill file or mark in drill legend
• Request cross-section verification on first article

How Atlas PCB Handles Back Drilling

Atlas PCB performs back drilling on high-layer-count boards from 8 to 68 layers, using X-ray-aligned CNC drilling with laser depth sensing. We routinely process backplanes and high-speed digital boards for data center, networking, and telecom applications.

Atlas PCB achieves ±4mil back drill depth tolerance with X-ray registration, supports single-side and dual-side back drilling, and provides cross-section verification on every first article. Every back-drilled order includes our 12-hour human engineering review — we verify stub lengths, anti-pad sizing, and back drill clearances against your signal integrity requirements before production.

For designs requiring tighter than ±4mil tolerance, we offer enhanced process control with 100% X-ray depth verification.

Summary

• Via stubs are unused through-hole via portions that resonate and destroy signals above 3-5GHz
• Back drilling removes the stub, leaving 5-10mil residual — the most cost-effective stub mitigation
• Required for 10G+ Ethernet, PCIe Gen4/5, 25G/56G/112G SerDes, high-speed backplanes
• Depth tolerance ±4mil is production standard; specify 5-10mil residual stub target
• Anti-pad sizing must account for larger back drill diameter + registration tolerance
• Always verify with cross-section on first article

Building a high-speed backplane or 10G+ design? Upload your Gerbers for a free engineering review — we will verify your back drill specifications, stub analysis, and signal integrity requirements.

Related guides: High-Speed PCB Design | Multilayer PCB Stackup Design Guide | Controlled Impedance PCB | HDI PCB Design Guide

Further Reading

• HDI PCB Technology: Microvias, Laser Drilling, and High-Density Design

• Blind Via vs Buried Via: Design Rules, Cost Impact & When to Use Each

• High-Speed PCB Design: Signal Integrity Essentials for Modern Electronics

• PCB Manufacturer with Engineering Review: Why Human DFM Audit Matters

• PCB DFM Checklist: 50 Points to Review Before Sending Gerbers