nearxos/ESP_Midea
1
0
Fork 0
Code Issues Pull Requests Actions Packages Projects Releases Wiki Activity
Files
a026f1fe6cd9ef0b1f7f46edeee2fca48cfd17da
ESP_Midea/Midea_ESP/TRACE_WIDTH_GUIDE.md
nearxos 473c4d11a7 test
2026-01-06 02:07:54 +02:00

6.4 KiB
Raw Blame History

Trace Width Guide: Power Distribution

Date: 2025-12-28
Based on: ESP32-WROOM-32E, AMS1117-3.3, TXB0104PWR

Current Requirements Summary

3.3V Power Rail

  • ESP32 peak current: 500mA (WiFi transmission)
  • LEDs (2×): ~12mA
  • TXB0104 VCCA: 5µA (negligible)
  • Pull-up resistors: <0.1mA (negligible)
  • Total peak current: ~512mA

5V Power Rail

  • TXB0104 VCCB: 5µA (negligible)
  • AC Connector: Minimal (if just signaling)
  • Total current: ~10mA (very low)

Trace Width Calculations

IPC-2221 Standard Reference

Current Carrying Capacity (10°C temperature rise):

Copper Weight Layer Type Capacity
1oz (35µm) External (F.Cu/B.Cu) ~1.0A per 1mm width
1oz (35µm) Internal ~0.5A per 1mm width
2oz (70µm) External ~2.0A per 1mm width
2oz (70µm) Internal ~1.0A per 1mm width

Recommended Trace Widths

For Standard 1oz Copper PCB (Most Common)

3.3V Power Traces

Minimum Requirements:

  • External layer: 0.51mm (for 512mA)
  • Internal layer: 1.02mm (for 512mA)

Recommended (with safety margin):

  • External layer: 1.0mm (50% margin, easy to route)
  • Internal layer: 1.5mm (50% margin)

Best Practice:

  • Main power rail: Use 1.0mm to 1.5mm wide traces
  • Branch traces: Can be narrower (0.5mm) for short runs to components
  • Copper zones/pours: Even better for power distribution

5V Power Traces

Minimum Requirements:

  • Any layer: 0.01mm (for 10mA) - theoretical minimum

Recommended:

  • Standard signal width: 0.3mm (sufficient and standard)
  • Main rail: 0.5mm (if using dedicated trace)

Note: 5V current is very low, so trace width is not critical. Use standard signal trace width (0.2-0.3mm) or slightly wider (0.5mm) for main rail.

Detailed Recommendations

3.3V Power Distribution

Option 1: Wide Traces (Recommended)

Main 3.3V rail:     1.0mm - 1.5mm width
Branch to ESP32:    0.8mm - 1.0mm width
Branch to LEDs:     0.3mm - 0.5mm width
Branch to TXB0104:  0.3mm - 0.5mm width

Option 2: Copper Zones/Pours (Best Practice)

  • Create a 3.3V copper zone covering the board area
  • Provides lowest impedance
  • Best for power distribution
  • Use 1.0mm clearance from other nets

Option 3: Hybrid Approach

  • Main rail: 1.5mm wide trace from regulator to ESP32 area
  • Copper zone: 3.3V zone around ESP32 and other components
  • Branch traces: 0.5mm for short connections

5V Power Distribution

Main 5V rail:       0.3mm - 0.5mm width (sufficient)
Branch to TXB0104:  0.3mm width (standard)
Branch to AC Conn:  0.3mm width (standard)

Note: 5V current is so low that trace width is not a concern. Use standard signal trace widths.

Implementation Guidelines

For KiCad PCB Layout

Setting Up Trace Widths

  1. Design Rules Setup:

    • Go to: File → Board Setup → Design Rules → Net Classes
    • Create net classes:
      • Power_3V3: Min width 0.5mm, Preferred 1.0mm, Max 2.0mm
      • Power_5V: Min width 0.2mm, Preferred 0.3mm, Max 1.0mm
      • Signal: Min width 0.2mm, Preferred 0.2mm, Max 0.5mm

  2. Assign Net Classes:

    • +3.3V net → Power_3V3 class
    • +5V net → Power_5V class
    • All other nets → Signal class

  3. Routing:

    • Route power traces first (widest)
    • Use copper zones for power distribution where possible
    • Keep power traces short and direct

Trace Width by Location

Location 3.3V Width 5V Width Notes
Regulator output 1.0-1.5mm - Main power source
To ESP32 VDD 1.0mm - High current path
To TXB0104 VCCA 0.5mm - Low current
To LEDs 0.3-0.5mm - Low current
To pull-ups 0.2-0.3mm - Very low current
5V main rail - 0.3-0.5mm Low current
To TXB0104 VCCB - 0.3mm Very low current

Copper Zone Recommendations

3.3V Copper Zone

  • Layer: F.Cu or B.Cu (or both)
  • Clearance: 0.5mm from other nets
  • Min width: 0.5mm (for narrow areas)
  • Coverage: Around ESP32, regulator, and power distribution area

GND Copper Zone

  • Layer: Both F.Cu and B.Cu (ground plane)
  • Clearance: 0.3mm from other nets
  • Coverage: Entire board (ground plane)
  • Vias: Connect both layers with multiple vias

5V Copper Zone (Optional)

  • Not necessary due to very low current
  • Can use if board space allows
  • Width: 0.3mm minimum if used

Thermal Considerations

Power Dissipation

  • 3.3V @ 512mA: ~1.69W (ESP32 peak)
  • Trace resistance: Lower with wider traces
  • Voltage drop: Minimize with wide traces and short paths

Trace Heating

With 1.0mm trace width and 512mA:

  • Temperature rise: ~10°C (acceptable)
  • Voltage drop: <50mV for typical trace lengths

Design Checklist

  • 3.3V main rail: 1.0mm minimum (1.5mm preferred)
  • 3.3V to ESP32: 1.0mm minimum
  • 3.3V branches: 0.5mm minimum for short runs
  • 5V traces: 0.3mm minimum (standard signal width)
  • Ground plane: Full coverage on one or both layers
  • Power zones: Consider copper zones for 3.3V
  • Vias: Use multiple vias for layer transitions on power nets
  • Clearance: Maintain proper clearance from other nets

Quick Reference

Minimum Trace Widths (1oz copper, external layer)

Net Current Minimum Recommended
+3.3V 512mA 0.51mm 1.0mm
+5V 10mA 0.01mm 0.3mm
GND - - Ground plane
Signals <10mA 0.2mm 0.2mm

Summary

  • 3.3V traces: Use 1.0mm width (or copper zone)
  • 5V traces: Use 0.3mm width (standard signal width)
  • GND: Use ground plane (copper zone covering entire board)

Additional Notes

Why 1.0mm for 3.3V?

  • Provides 50% safety margin over minimum requirement
  • Easy to route and manufacture
  • Low voltage drop
  • Good thermal performance
  • Standard practice for power traces

Why 0.3mm for 5V?

  • Current is very low (10mA)
  • Standard signal trace width
  • Easy to route
  • Sufficient for the application

Copper Zones vs Traces

  • Copper zones: Best for power distribution (lowest impedance)
  • Traces: Good for point-to-point connections
  • Hybrid: Use zones for main distribution, traces for branches

Guide created: 2025-12-28