Internal vs External PCB Layers
Every multilayer PCB has internal and external layers, but they're not interchangeable. Where you place your traces—on an outer layer or buried inside—affects everything from current capacity to impedance to thermal performance. Understanding these differences is essential for effective PCB design.
This guide explains when to use each layer type, with practical guidelines for power traces, high-speed signals, and thermal management.
External vs Internal: The Basics
External Layers (Top/Bottom)
The outer layers of the PCB, exposed to air (with solder mask on top). Components are mounted here, and traces have access to convection cooling.
- Direct component access
- Better heat dissipation
- Higher current capacity
- Easier to probe/debug
Internal Layers (Inner)
Layers sandwiched between the outer layers, surrounded by FR4 dielectric material. No direct component access, heat must conduct through FR4.
- Protected from environment
- Natural shielding (if planes)
- Lower current capacity
- Better for controlled impedance
Typical Layer Stackup
This is a standard 4-layer stackup. 6-layer and 8-layer boards add more signal layers between the planes.
Current Capacity: The Big Difference
The most significant difference between internal and external layers is current capacity. Because internal layers can't dissipate heat as effectively, they require wider traces for the same current.
| Current | External Width | Internal Width | Increase |
|---|---|---|---|
| 1 A | 10 mil | 25 mil | 150% |
| 2 A | 30 mil | 75 mil | 150% |
| 3 A | 55 mil | 140 mil | 155% |
| 5 A | 110 mil | 280 mil | 155% |
| 10 A | 330 mil | 850 mil | 158% |
Key Takeaway: Internal traces need roughly 2.5× the width of external traces for the same current capacity. This comes from the IPC-2221 constants: k=0.024 for internal vs k=0.048 for external.
Use our Trace Width Calculator to get exact values for your specific requirements—it automatically accounts for layer type.
Why Internal Layers Have Lower Capacity
It all comes down to thermal conductivity. FR4 is a poor thermal conductor compared to air.
| Material | Thermal Conductivity (W/m·K) |
|---|---|
| Copper | 385 |
| Air (still) | 0.026 |
| FR4 | 0.25 - 0.3 |
Wait—FR4 is actually better than air? Yes, but there's a catch:
External Layer Heat Path:
Trace → Air (convection) + Radiation → Environment
Convection and radiation are very efficient. Even still air provides good cooling through natural convection currents.
Internal Layer Heat Path:
Trace → FR4 (conduction) → External copper → Air/Radiation
Heat must conduct through FR4 to reach the surface. FR4's low thermal conductivity creates a thermal bottleneck.
When to Use Each Layer Type
Use External Layers For:
- High-current traces (power input, motor drivers, LED drivers)
- Component connections (obvious—components mount here)
- Heat-dissipating traces (thermal pads, power transistors)
- Test points and probing access
- RF traces with coplanar waveguide structure
Use Internal Layers For:
- Power and ground planes (low impedance distribution)
- Shielded signal routing (stripline for EMI-sensitive signals)
- High-speed differential pairs (better crosstalk isolation)
- Dense routing (when outer layers are full)
- Reference planes for controlled impedance
| Application | Preferred Layer | Reason |
|---|---|---|
| Power input (>1A) | External | Current capacity |
| Ground plane | Internal | Reference for signals |
| USB 3.0 data | Either (stripline preferred) | EMI shielding |
| DDR data lines | External (microstrip) | Component proximity |
| Analog signals | Internal (stripline) | Noise immunity |
| LED driver traces | External | Current + thermal |
Impedance Differences
Layer type affects controlled impedance design because the dielectric environment differs:
| Structure | Layer Type | Trace Width | Effective εᵣ |
|---|---|---|---|
| Microstrip | External | 15 mil | ~3.2 |
| Stripline | Internal | 5 mil | ~4.3 |
Notice that stripline traces are narrower than microstrip for the same impedance. This is because:
- Stripline is fully embedded in dielectric (higher effective εᵣ)
- Has reference planes above and below (more capacitance)
- No air interface to reduce effective dielectric constant
For more on transmission line structures, see our Microstrip vs Stripline Guide.
Thermal Via Strategy for Internal Layers
If you must route power on internal layers (sometimes unavoidable), you can improve thermal performance with strategic via placement:
1. Add Thermal Vias
Place thermal vias from internal power traces to external copper pours. This creates a heat path through the board.
2. Connect to Ground/Power Planes
Large copper planes on adjacent layers act as heat spreaders. Ensure good via connections to these planes.
3. Use Copper Pours
Even on signal layers, copper pours connected to ground or power can help spread heat from high-current traces.
For more thermal via guidance, see our Thermal Via vs Signal Via Guide.
EMI and Shielding Considerations
Internal layers offer natural EMI shielding when used as planes or for stripline routing:
| Configuration | EMI Emission | EMI Immunity |
|---|---|---|
| Microstrip (external) | Higher | Lower |
| Stripline (internal) | Very Low | High |
| CPWG (external) | Medium | Medium-High |
Design Tip: For EMI-sensitive designs, route high-speed signals on internal layers between ground planes (stripline). The planes act as a Faraday cage, containing emissions and blocking external interference.
Practical Layer Assignment Flow
Assign Power and Ground Planes
Usually internal layers 2 and 3 in a 4-layer board. These provide low-impedance power distribution and reference planes.
Route High-Current Traces Externally
Place power input traces, motor drivers, and any trace >1A on external layers for better thermal performance.
Decide High-Speed Signal Strategy
Choose microstrip (external) or stripline (internal) based on EMI requirements and component access needs.
Fill Remaining Routing Needs
Use remaining layer capacity for general signal routing, ensuring proper reference plane continuity.
Summary
| Aspect | External | Internal |
|---|---|---|
| Current capacity | Higher (baseline) | Lower (~40% of external) |
| Heat dissipation | Good (convection) | Poor (conduction only) |
| Component access | Direct | Via required |
| EMI shielding | None | Excellent (if planes) |
| Impedance control | Microstrip | Stripline |
| Trace width (50Ω) | Wider | Narrower |
The key takeaway: use external layers for power and thermal-critical traces, and internal layers for EMI-sensitive signals and reference planes. When calculating trace widths, always select the correct layer type—the difference is significant.
Calculate your trace widths with the correct layer setting using our free PCB Trace Width Calculator.
Related Reading
Related Tools & Calculators
Related Articles
Try Our Free Calculators
Put this knowledge into practice with our IPC-compliant PCB design tools.