Impedance control is critical for any PCB carrying high-speed signals — USB, HDMI, Ethernet, DDR memory, and RF circuits all require specific trace impedances to function reliably. In India, most standard PCB fabricators offer controlled impedance as an add-on service, typically adding 15-30% to the base fabrication cost. This guide explains how impedance works, how to design 50-ohm single-ended and 90-ohm differential pair traces, and what to specify when ordering from your manufacturer.
Table of Contents
- Impedance Basics for PCB Designers
- Microstrip Trace Design
- Stripline Trace Design
- Differential Pair Routing
- Stack-Up Planning for Impedance
- Using Impedance Calculators
- Manufacturing Tolerances
- Frequently Asked Questions
Impedance Basics for PCB Designers
Characteristic impedance is the ratio of voltage to current for a signal wave travelling along a transmission line. It depends on four physical factors:
- Trace width (w): Wider traces have lower impedance
- Dielectric thickness (h): Distance between trace and reference plane — thicker dielectric means higher impedance
- Dielectric constant (Er): FR-4 is typically 4.2-4.6 at 1 GHz — higher Er means lower impedance
- Copper thickness (t): Standard 1oz (35µm) — thicker copper slightly lowers impedance
When a signal’s rise time is fast enough that the trace length exceeds roughly 1/6 of the signal wavelength, the trace behaves as a transmission line and impedance matching becomes necessary. For a typical FR-4 PCB, this happens at trace lengths above approximately 25mm for USB 2.0 signals and above 10mm for USB 3.0.
Microstrip Trace Design
A microstrip is a trace on an outer layer with a reference (ground) plane on the adjacent inner layer. This is the most common configuration for controlled impedance.
| Target Impedance | FR-4 (Er=4.3), 1oz Cu, Standard Stackup |
|---|---|
| 50 Ohm single-ended | ~0.28mm trace width over 0.2mm dielectric (4-layer) or ~0.18mm over 0.1mm |
| 75 Ohm single-ended | ~0.15mm trace width over 0.2mm dielectric |
| 90 Ohm differential | ~0.15mm trace width, 0.2mm gap, over 0.2mm dielectric |
| 100 Ohm differential | ~0.12mm trace width, 0.2mm gap, over 0.2mm dielectric |
These are approximate values — always use a field solver (not simplified formulas) for production designs. The trace width varies significantly with the actual dielectric thickness and Er value of your specific laminate.
Stripline Trace Design
A stripline is a trace on an inner layer sandwiched between two reference planes. Striplines offer better EMI performance because the signal is fully shielded, but they require more layers (minimum 4-layer board).
- Stripline impedance is lower than microstrip for the same trace width because the trace is surrounded by dielectric on all sides
- For 50 Ohm stripline in standard FR-4: trace width is typically 0.15-0.2mm between two planes spaced 0.4mm apart
- Signal propagation is slower in stripline (about 50% of free-space velocity vs 60% for microstrip)
- Use stripline for high-speed buses that need EMI containment: DDR data lines, PCIe, SATA
Differential Pair Routing
Differential pairs carry complementary signals (D+ and D-) and require matched impedance, length, and spacing. Common differential impedance targets:
| Interface | Differential Impedance | Tolerance |
|---|---|---|
| USB 2.0 | 90 Ohm | ±10% |
| USB 3.0/3.1 | 90 Ohm | ±7% |
| HDMI | 100 Ohm | ±10% |
| Ethernet (100BASE-TX) | 100 Ohm | ±10% |
| PCIe | 85 Ohm | ±10% |
| LVDS | 100 Ohm | ±10% |
Key routing rules for differential pairs:
- Maintain constant spacing between the two traces throughout the route
- Length-match both traces to within 0.1mm (5 mils) for USB, tighter for higher speeds
- Avoid routing differential pairs near board edges or over split planes
- Keep other traces at least 3x the pair spacing away to avoid crosstalk
- When a pair must change layers, place vias for both traces side by side with identical via structures
Stack-Up Planning for Impedance
The PCB stack-up determines what impedance values are achievable. Work with your fabricator to finalise the stack-up before routing.
Standard 4-layer stack-up for impedance control:
| Layer | Function | Thickness |
|---|---|---|
| L1 (Top) | Signal + Components | 35µm Cu |
| Prepreg | Dielectric | 0.2mm (7628 prepreg) |
| L2 | Ground Plane | 35µm Cu |
| Core | Dielectric | 1.0mm |
| L3 | Power Plane | 35µm Cu |
| Prepreg | Dielectric | 0.2mm |
| L4 (Bottom) | Signal + Components | 35µm Cu |
The thin 0.2mm prepreg between L1/L2 (and L3/L4) enables practical trace widths for 50-ohm microstrip. If the dielectric is too thick (e.g., 0.5mm), the required trace width becomes very wide and wastes routing space.
Using Impedance Calculators
Always use a 2D field solver rather than simplified empirical formulas. Recommended free tools:
- Saturn PCB Toolkit: Free Windows application with microstrip, stripline, and differential pair calculators. Uses the IPC-2141 equations
- KiCad built-in calculator: Tools → PCB Calculator → Transmission Line tab. Supports microstrip and stripline
- JLCPCB impedance calculator: Online tool at their website, pre-loaded with their actual laminate parameters
- Altium/Mentor field solvers: More accurate 2D electromagnetic solvers in professional EDA tools
When using any calculator, input your manufacturer’s actual laminate data (Er, loss tangent, prepreg thickness) rather than generic FR-4 values. Ask your fabricator for their stack-up document.
Manufacturing Tolerances
Indian PCB manufacturers typically guarantee impedance within ±10% of the target value. Achieving tighter tolerance (±5% or ±7%) requires:
- Specifying controlled impedance on your fab drawing with target values and tolerance
- Using the manufacturer’s recommended stack-up (they know their material Dk values)
- TDR (Time Domain Reflectometry) testing — the manufacturer measures actual impedance on test coupons built into the panel rail
- Consistent trace widths — avoid necking down impedance-controlled traces at component pads
The main cost driver is the TDR testing and the need for the manufacturer to adjust trace widths based on their actual etching process. Budget PCB services (under ₹500 per panel) typically do not offer controlled impedance.
Frequently Asked Questions
Do I need impedance control for a 2-layer board?
It is possible but difficult. A 2-layer board with 1.6mm thickness requires very wide traces (~3mm) for 50 ohms because the dielectric is thick. For USB or HDMI signals, use a 4-layer board with thin prepreg. For UART or I2C at moderate speeds, 2-layer boards work fine without impedance control.
What happens if impedance is wrong?
Signal reflections occur at impedance mismatches, causing ringing, overshoot, and data errors. USB devices may fail enumeration, HDMI may show sparkles or no output, and DDR memory may produce random bit errors. The severity depends on how far off the impedance is and the signal frequency.
Can JLCPCB and PCBWay do controlled impedance?
Yes, both offer controlled impedance at additional cost (approximately $5-15 extra per order). Specify the target impedance, layer, and tolerance in your order notes. They will adjust trace widths during CAM processing and include TDR test coupons.
How do I specify impedance on my Gerber files?
Impedance is specified in the fabrication drawing (fab note), not in the Gerber data. Include a table listing: layer, trace type (microstrip/stripline/differential), target impedance, tolerance, trace width, and spacing. Also include your desired stack-up for reference.
Does solder mask affect impedance?
Yes, solder mask has a dielectric constant of approximately 3.5 and adds a coating over outer-layer traces. This typically lowers microstrip impedance by 2-3 ohms. Professional impedance calculators include a solder mask parameter. For ±10% tolerance this effect is usually within margin, but for ±5% tolerance it matters.
Find prototyping boards, measurement instruments, and PCB supplies for your impedance-controlled designs at Zbotic PCB & Prototyping — shipping across India.
Add comment