10 Common PCB Trace Width Mistakes
You've spent hours perfecting your schematic, placed your components just right, and you're about to start routing. Then it hits you: "What trace width should I use?" Get it wrong, and you could end up with a board that overheats, fails in the field, or simply doesn't work at all.
After reviewing thousands of PCB designs (and making plenty of mistakes ourselves), we've compiled the 10 most common trace width errors engineers make—and how to avoid them. Some are obvious, others are subtle. All of them can ruin your day.
Mistake #1: Using the Same Width for Everything
The classic rookie mistake: setting your design rules to 10-mil traces and calling it a day. Yes, it's easier. No, it won't work for anything beyond the simplest designs.
The Problem: A 10-mil trace on 1oz copper can only handle about 0.5A with a 10°C temperature rise. Your 5V/2A power input? That needs at least 50 mils—five times wider.
The Fix: Create multiple net classes in your EDA tool:
- Signal nets: 5-8 mil (low-current logic)
- Power nets: Calculate based on current using a trace width calculator
- High-speed nets: Impedance-controlled width
| Net Type | Typical Current | Min Width (1oz) |
|---|---|---|
| Digital signals | <100 mA | 5-8 mil |
| Analog signals | <50 mA | 8-12 mil |
| LED drivers | 20-100 mA | 10-15 mil |
| Motor control | 1-5 A | 50-150 mil |
| Power input | Varies | Calculate! |
Mistake #2: Ignoring Temperature Rise
"The calculator says 30 mil is fine for 3A." Sure, but at what temperature rise? Many engineers grab the first number from a calculator without checking the thermal assumptions.
The Problem: A trace width calculated for 20°C rise will get hot—really hot. In an enclosed product with poor ventilation, that rise stacks on top of ambient temperature. If your ambient is 40°C and you add 20°C rise, your trace is running at 60°C.
| Temp Rise | Trace Width | Actual Trace Temp (40°C ambient) |
|---|---|---|
| 5°C | 95 mil | 45°C |
| 10°C | 55 mil | 50°C |
| 20°C | 32 mil | 60°C |
| 30°C | 24 mil | 70°C |
The Fix: Design for 10°C rise as your default. Only go higher (15-20°C) if you know the thermal environment can handle it. For safety-critical or enclosed products, consider 5°C rise.
Mistake #3: Confusing Internal and External Layers
Internal layers conduct heat poorly because they're sandwiched in FR4, which is basically a thermal insulator. Using external layer calculations for internal traces is a recipe for thermal failure.
The Problem: An internal trace needs roughly 2× the width of an external trace to carry the same current safely. IPC-2221 uses k=0.024 for internal vs k=0.048 for external—that's half the current capacity for the same cross-section.
| Layer Type | Required Width | Heat Dissipation |
|---|---|---|
| External (Top/Bottom) | 110 mil | Convection + radiation |
| Internal (Embedded) | 280 mil | Conduction through FR4 only |
The Fix: Always route high-current traces on external layers when possible. If you must use internal layers, recalculate with the internal layer option selected—our calculator handles this automatically. Learn more in our Internal vs External Layers Guide.
Mistake #4: Forgetting About Manufacturing Tolerances
Your design says 10 mil, but what does the actual board say? PCB manufacturing has tolerances, and etching can remove copper from trace edges.
The Problem: Typical trace width tolerance is ±20% for standard processes. Your 10-mil trace could end up as 8 mil—a 36% reduction in cross-sectional area and current capacity.
| Design Width | Worst Case (-20%) | Current Capacity Loss |
|---|---|---|
| 5 mil | 4 mil | ~30% |
| 10 mil | 8 mil | ~25% |
| 20 mil | 16 mil | ~22% |
| 50 mil | 40 mil | ~20% |
The Fix: Add a 10-20% margin to your calculated trace widths, especially for critical power traces. If your calculation says 50 mil, design for 55-60 mil. Better yet, ask your fab house for their specific tolerances.
Mistake #5: Not Accounting for Voltage Drop
Trace width calculations focus on heating, but voltage drop can kill your design even if thermals are fine—especially in low-voltage systems.
The Problem: A 3.3V system with 100mV of voltage drop just lost 3% of its supply. For a sensitive MCU or sensor, that might push you outside the operating voltage range or cause noise issues.
| Supply | V-Drop (50 mil) | % Loss | Acceptable? |
|---|---|---|---|
| 24V | 120 mV | 0.5% | ✓ Yes |
| 12V | 120 mV | 1.0% | ✓ Yes |
| 5V | 120 mV | 2.4% | ⚠ Marginal |
| 3.3V | 120 mV | 3.6% | ✗ Problem |
| 1.8V | 120 mV | 6.7% | ✗✗ Critical |
The Fix: Calculate voltage drop, not just temperature rise. For low-voltage rails (<5V), target <1% drop. Use wider traces or heavier copper. Our calculator shows voltage drop alongside trace width.
Mistake #6: Necking Down at Vias
You've got a beautiful 100-mil power trace... that necks down to 20 mil at every via transition. Congratulations, you just created a bottleneck.
The Problem: Current density at the necked portion can be 5× higher than the rest of the trace. This creates a hot spot that can lead to trace failure or solder joint damage.
The Fix: Use multiple vias in parallel to share the current. For high-current transitions, use via arrays. See our Via Sizing Guide and Via Current Calculator to determine how many vias you need.
| Current | Single Via (10 mil) | Recommended |
|---|---|---|
| 1 A | ❌ 0.8A capacity | 2 vias |
| 3 A | ❌ 0.8A capacity | 5-6 vias |
| 5 A | ❌ 0.8A capacity | 8-10 vias |
| 10 A | ❌ 0.8A capacity | 15-20 vias |
Mistake #7: Using Wrong Copper Weight
Calculating trace width for 1oz copper and then sending your board out with 0.5oz default? You just halved your current capacity.
The Problem: Many engineers don't specify copper weight in their fab notes, assuming they'll get 1oz. Some budget fabs default to 0.5oz or even 1/3oz on internal layers.
| Copper | Required Width | If You Assumed 1oz... |
|---|---|---|
| 0.5 oz | 110 mil | Design undersized by 2× |
| 1 oz | 55 mil | (Correct) |
| 2 oz | 28 mil | Over-designed but safe |
The Fix: Always specify copper weight in your fab notes and verify it matches your calculations. Read our Copper Weight Comparison Guide for detailed information.
Mistake #8: Ignoring Return Current Path
You calculated the power trace width perfectly. But what about the return path? Current doesn't magically teleport back to the source—it needs a trace too.
The Problem: Many designs have wide power traces but thin ground connections. The current is the same in both directions! If your VCC trace is 100 mil but GND is routing through a via array to a ground plane with a bottleneck, you've got a weak link.
The Fix: Always size the return path (GND) equal to or larger than the supply path. For ground planes, ensure vias and connections to the plane can handle the current. Copper pours help, but verify they provide a continuous low-impedance path.
Mistake #9: Using Outdated Standards
"I've been using this trace width chart since college." Great—how old is that chart, and does it account for modern PCB construction?
The Problem: IPC-2221 charts are based on 1950s data. While still useful for conservative estimates, they don't account for modern manufacturing practices, copper planes, or thermal management techniques.
The Fix: Use IPC-2152 for more accurate results, especially if you have copper planes nearby. Understand the differences between standards—read our IPC-2221 vs IPC-2152 comparison.
Mistake #10: Not Testing Under Real Conditions
Your trace width calculations assume certain conditions. But does your actual product operate under those conditions?
The Problem: Calculations assume:
- Still air (no forced convection)
- Isolated traces (no adjacent heat sources)
- Steady-state current (no transients)
- Room temperature ambient
Real products have enclosures, neighboring hot components, pulsed currents, and varying ambient temperatures.
The Fix: Test prototypes with a thermal camera under worst-case conditions. Measure actual trace temperatures during full-load operation. Add margin (20-30%) if testing isn't possible before production.
Quick Reference Checklist
| # | Check Item | Action |
|---|---|---|
| 1 | Multiple trace widths | Create net classes |
| 2 | Temperature rise | Design for 10°C default |
| 3 | Layer type | Select internal/external |
| 4 | Manufacturing tolerance | Add 10-20% margin |
| 5 | Voltage drop | Calculate for <1% on low-V |
| 6 | Via transitions | Use multiple vias |
| 7 | Copper weight | Verify in fab notes |
| 8 | Return path | Size GND = VCC |
| 9 | Standards used | Consider IPC-2152 |
| 10 | Real-world testing | Thermal camera check |
The Bottom Line
Trace width design isn't rocket science, but it does require attention to detail. The biggest mistakes come from assumptions—assuming default copper weight, assuming external layer calculations apply to internal layers, assuming the numbers from a calculator are final without considering real-world factors.
Use our PCB Trace Width Calculator as a starting point, add appropriate margins, and verify with testing when possible. Your future self (and your customers) will thank you.
Free Tools to Help
Related Reading
Related Tools & Calculators
Related Articles
Try Our Free Calculators
Put this knowledge into practice with our IPC-compliant PCB design tools.