ESP_Midea/Midea_ESP/QUICK_START_SCHEMATIC.md

Quick Start: Building the Schematic

Step-by-Step Guide

1. Start with Power Supply (Page 1 or Top Left)

Add Components:

1. Press A → Search Midea_ESP:AMS1117-3.3 → Place as U1
2. Press A → Search Device:C → Place 4 capacitors: C1, C2, C3, C4

Set Values:

• C1, C2: 10µF
• C3, C4: 100nF

Add Power Symbols:

• Press P → Select +3V3 → Place near U1 output
• Press P → Select +5V → Place near where J1 will connect (on Page 3)
• Press P → Select GND → Place multiple times

Connect:

• Net Label +5V_POWER → U1 Pin 3 (IN) (this connects to J1 Pin 1 on Page 3)
• Net Label +5V_POWER → C1 (one terminal) (parallel - connect directly to +5V net)
• Net Label +5V_POWER → C3 (one terminal) (parallel - connect directly to +5V net)
• C1 (other terminal) → GND
• C3 (other terminal) → GND
• U1 Pin 2 (OUT) → +3V3 power symbol (connect to +3V3 net)
• U1 Pin 2 (OUT) → C2 (one terminal) (parallel - connect directly to +3V3 net)
• U1 Pin 2 (OUT) → C4 (one terminal) (parallel - connect directly to +3V3 net)
• C2 (other terminal) → GND
• C4 (other terminal) → GND
• U1 Pin 1 (GND) → GND
• U1 Pin TAB (GND) → GND

Note:

• Power comes from J1 Pin 1 (+5V) on Page 3. Use net labels to connect between pages.
• C1 and C3 are in PARALLEL (both connected between +5V and GND for input filtering)
• C2 and C4 are in PARALLEL (both connected between +3V3 and GND for output filtering)

---

2. Add ESP32 (Page 2 or Center)

Add Components:

1. Press A → Search Midea_ESP:ESP32-WROOM-32E → Place as U2
2. Press A → Search Device:C → Place 2 capacitors: C5 (100nF), C6 (10µF)
3. Press A → Search Button_Switch_SMD:SW_PUSH → Place 2 buttons: SW1, SW2
4. Press A → Search Device:R → Place 4 resistors: R1, R2, R3, R4
5. Press A → Search Device:LED → Place 2 LEDs: LED1, LED2

Set Values:

• R1, R2: 220Ω
• R3, R4: 10kΩ
• C5: 100nF
• C6: 10µF

Connect Power:

• U2 Pin 2 (VDD) → +3V3 (only exposed VDD pin on your module)
• U2 Pin 2 (VDD) → C5 (one terminal) → +3V3, C5 (other terminal) → GND (100nF decoupling)
• U2 Pin 2 (VDD) → C6 (one terminal) → +3V3, C6 (other terminal) → GND (10µF bulk capacitor)
• All exposed U2 GND pins → GND (typically Pin 1 and other exposed GND pins)

Connect Buttons:

• SW1 Pin 1 → U2.EN, R3 → +3V3
• SW1 Pin 2 → GND
• SW2 Pin 1 → U2.GPIO0, R4 → +3V3
• SW2 Pin 2 → GND

Connect LEDs:

• LED1 Anode → R1 → U2.GPIO2
• LED1 Cathode → GND
• LED2 Anode → R2 → U2.GPIO4
• LED2 Cathode → GND

Add Net Labels:

• Press L → Type ESP32_TX → Attach to wire from U2.GPIO17
• Press L → Type ESP32_RX → Attach to wire from U2.GPIO16

---

3. Add Level Shifter and AC Connector (Page 3 or Right)

Add Components:

1. Press A → Search Midea_ESP:TXB0104PWR → Place as U3
2. Press A → Search Connector_JST:JST_XH_B4B-XH-A → Place as J1

Connect Power:

• U3 Pin 12 (VCCA) → +3V3
• U3 Pin 11 (VCCB) → +5V
• U3 Pin 10 (OE) → +3V3
• U3 Pins 5, 13, 14 (GND) → GND

Connect Signals:

• U3 Pin 1 (A1) → Net Label ESP32_TX (connects to U2.GPIO17)
• U3 Pin 2 (A2) → Net Label ESP32_RX (connects to U2.GPIO16)
• U3 Pin 9 (B1) → Net Label AC_RX → J1 Pin 2
• U3 Pin 8 (B2) → Net Label AC_TX → J1 Pin 3
• J1 Pin 1 → Net Label +5V_POWER → Connect to Page 1 (U1 input via capacitors)
• J1 Pin 4 → GND

Note: J1 is a JST-XH connector on the PCB. This connector provides:

• Power input (Pin 1: +5V) - Powers the entire PCB
• AC communication (Pins 2-3: UART signals)
• Ground (Pin 4: GND)

Connect a cable with matching JST-XH connector to your AC unit.

---

4. Add Programming Header (Required - Page 4 or Bottom)

Add Components:

1. Press A → Search Connector_PinHeader_2.54mm:PinHeader_2x04_P2.54mm_Vertical → Place as J2
2. Press A → Search Device:R → Place 2 resistors: R5, R6 (optional)

Set Values:

• R5, R6: 10kΩ (optional - for pull-ups)

Connect:

• J2 Pin 1 → +3V3 (optional - for powering from programmer)
• J2 Pin 2 → GND
• J2 Pin 3 → Net Label UART_TX (connects to U2.GPIO1)
• J2 Pin 4 → Net Label UART_RX (connects to U2.GPIO3)
• J2 Pin 5 → Net Label DTR → U2.GPIO0 (auto-reset)
• J2 Pin 6 → Net Label RTS → U2.EN (auto-reset)

Optional Pull-ups (for reliability):

• J2 Pin 5 (DTR) → R5 → +3V3
• J2 Pin 6 (RTS) → R6 → +3V3

Add Net Labels on Page 2:

• Press L → Type UART_TX → Attach to wire from U2.GPIO1
• Press L → Type UART_RX → Attach to wire from U2.GPIO3
• Press L → Type DTR → Attach to wire from U2.GPIO0
• Press L → Type RTS → Attach to wire from U2.EN

Programming Header Pinout (J2) - 2x4 Header:

Top Row:    Pin 1: VCC  Pin 2: GND  Pin 3: TX   Pin 4: RX
Bottom Row: Pin 5: DTR  Pin 6: RTS  Pin 7: NC   Pin 8: NC

Pin 1: +3V3 (optional)
Pin 2: GND
Pin 3: UART_TX (ESP32 TX → Programmer RX)
Pin 4: UART_RX (ESP32 RX ← Programmer TX)
Pin 5: DTR (Auto-reset)
Pin 6: RTS (Auto-reset)

External USB-to-Serial Adapter Connection: When flashing, connect your USB-to-Serial adapter (CP2102, CH340, FT232, etc.):

• Adapter VCC → J2 Pin 1 (optional - only if powering ESP32 from adapter)
• Adapter GND → J2 Pin 2
• Adapter RX → J2 Pin 3 (receives TX from ESP32)
• Adapter TX → J2 Pin 4 (sends to RX of ESP32)
• Adapter DTR → J2 Pin 5 (auto-reset)
• Adapter RTS → J2 Pin 6 (auto-reset)

---

Keyboard Shortcuts

• A - Add Symbol
• W - Add Wire
• P - Add Power Port
• L - Add Net Label
• E - Edit Component
• M - Move Component
• R - Rotate Component
• Delete - Delete Selected
• Ctrl+Z - Undo
• Ctrl+S - Save

---

Verification Checklist

After completing the schematic:

• All components have reference designators (U1, U2, etc.)
• All components have values set
• All power pins connected to appropriate power rails
• All ground pins connected to GND
• Net labels match between pages (if using multiple pages)
• No unconnected pins (except NC pins)
• Run ERC: Tools → Electrical Rules Checker
• Fix any ERC warnings/errors

---

Common Issues

1. "Unconnected pin" warning: Check if pin should be connected or marked as NC
2. "Power pin not driven": Ensure power symbols are connected
3. "Multiple net names": Check for duplicate net labels or conflicting connections
4. "Pin connected to multiple nets": Check for wiring errors