Initial KiCad project

2026-01-04 01:19:56 +02:00
commit 8a26f501d8
45 changed files with 133173 additions and 0 deletions
--- a/Midea_ESP/SCHEMATIC_COMPONENT_LIST.md
+++ b/Midea_ESP/SCHEMATIC_COMPONENT_LIST.md
@@ -0,0 +1,451 @@
+# Schematic Component List and Connection Guide
+
+## Schematic Structure (Recommended)
+
+### Page 1: Power Supply Section
+- Power input via JST connector (J1 Pin 1)
+- Voltage regulator (AMS1117-3.3)
+- Input/output capacitors
+- Power distribution
+
+### Page 2: Main Controller (ESP32)
+- ESP32-WROOM-32E module
+- Decoupling capacitors
+- Reset and boot buttons
+- Status LEDs
+
+### Page 3: Level Shifter and AC Interface
+- TXB0104 level shifter
+- AC connector (JST-XH)
+- Signal connections
+
+### Page 4: Programming Header (Optional)
+- Header pins for external USB-to-Serial adapter
+- Auto-reset connections
+
+---
+
+## Component List
+
+### Page 1: Power Supply
+
+| Ref | Component | Library | Symbol | Value | Notes |
+|-----|-----------|---------|--------|-------|-------|
+| U1 | Voltage Regulator | `Midea_ESP` | `AMS1117-3.3` | AMS1117-3.3 | 3.3V regulator |
+| C1 | Capacitor | `Device` | `C` | 10µF | Input capacitor |
+| C2 | Capacitor | `Device` | `C` | 10µF | Output capacitor |
+| C3 | Capacitor | `Device` | `C` | 100nF | Input decoupling |
+| C4 | Capacitor | `Device` | `C` | 100nF | Output decoupling |
+
+**Note:** Power is supplied via J1 Pin 1 (+5V) from the AC unit connection. See Page 3 for J1 connector details.
+
+**Connections:**
+- **J1 Pin 1 (+5V)** → **U1 Pin 3 (IN)** (connect from Page 3 using net label `+5V_POWER`)
+- **J1 Pin 1 (+5V)** → **C1 (one terminal)** (parallel connection - connect directly to +5V net)
+- **J1 Pin 1 (+5V)** → **C3 (one terminal)** (parallel connection - connect directly to +5V net)
+- **C1 (other terminal)** → **GND**
+- **C3 (other terminal)** → **GND**
+- **U1 Pin 2 (OUT)** → **+3V3 Power Rail** (connect to +3V3 power symbol)
+- **U1 Pin 2 (OUT)** → **C2 (one terminal)** (parallel connection - connect directly to +3V3 net)
+- **U1 Pin 2 (OUT)** → **C4 (one terminal)** (parallel connection - connect directly to +3V3 net)
+- **C2 (other terminal)** → **GND**
+- **C4 (other terminal)** → **GND**
+- **U1 Pin 1 (GND)** → **GND**
+- **U1 Pin TAB (GND)** → **GND**
+- **J1 Pin 4 (GND)** → **GND** (connect from Page 3)
+
+**Note:** 
+- All capacitors are unpolarized (ceramic), so either terminal can connect to either net.
+- **C1 and C3 are in PARALLEL** between +5V and GND (input filtering/decoupling)
+- **C2 and C4 are in PARALLEL** between +3V3 and GND (output filtering/decoupling)
+
+**Power Symbols:**
+- Add `+3V3` power symbol (press `P`, select `+3V3`)
+- Add `GND` power symbol (press `P`, select `GND`)
+- Add `+5V` power symbol (press `P`, select `+5V`) - connects to J1 Pin 1 and level shifter
+
+---
+
+### Page 2: ESP32 Main Controller
+
+| Ref | Component | Library | Symbol | Value | Notes |
+|-----|-----------|---------|--------|-------|-------|
+| U2 | ESP32 Module | `Midea_ESP` | `ESP32-WROOM-32E` | ESP32-WROOM-32E | Main MCU (onboard antenna) |
+| C5 | Capacitor | `Device` | `C` | 100nF | VDD decoupling (Pin 2) |
+| C6 | Capacitor | `Device` | `C` | 10µF | Bulk capacitor near module |
+| SW1 | Reset Button | `Button_Switch_SMD` | `SW_PUSH` | - | Reset switch |
+| SW2 | Boot Button | `Button_Switch_SMD` | `SW_PUSH` | - | Boot/Flash switch |
+| R3 | Resistor | `Device` | `R` | 10kΩ | Reset pull-up |
+| R4 | Resistor | `Device` | `R` | 10kΩ | Boot pull-up |
+| LED1 | LED | `Device` | `LED` | - | WiFi status |
+| LED2 | LED | `Device` | `LED` | - | BLE status |
+| R1 | Resistor | `Device` | `R` | 220Ω | LED1 current limit |
+| R2 | Resistor | `Device` | `R` | 220Ω | LED2 current limit |
+
+**Power Connections (For ESP32-WROOM-32E with Only Pin 2 VDD Exposed):**
+- **ESP32 Pin 2 (VDD)** → **+3V3 Power Rail**
+  - **Note:** Only Pin 2 (VDD) is exposed on your module (onboard antenna variant)
+  - **C5 (100nF):** **U2 Pin 2 (VDD)** → **C5 (one terminal)** → **+3V3**, **C5 (other terminal)** → **GND** (decoupling capacitor - required)
+  - **C6 (10µF):** **U2 Pin 2 (VDD)** → **C6 (one terminal)** → **+3V3**, **C6 (other terminal)** → **GND** (bulk capacitor - recommended near module)
+  - **Placement:** C5 and C6 must be placed as close as possible to Pin 2 (<5mm recommended)
+- **ESP32 GND pins** (all exposed GND pins) → **GND**
+  - **Note:** Connect all exposed GND pins to ground plane
+  - **Typical GND pins:** Pin 1, and any other exposed GND pins on your module
+- **Note:** Internal VDD pins are handled by the module internally - only external Pin 2 needs decoupling
+
+**Critical Control Pins (Per Datasheet):**
+- **U2 EN (Enable Pin) - Pin 3 in RF_Module library:**
+  - **Function:** Active HIGH - enables ESP32 operation (must be HIGH for normal operation)
+  - **Pull-up resistor:** R3 (10kΩ) → +3V3 (required by datasheet)
+  - **Reset button:** SW1 connected to EN pin (active LOW reset - pulls EN LOW to reset)
+  - **Connections:**
+    - **U2.EN** → **R3 (10kΩ)** → **+3V3** (pull-up resistor)
+    - **U2.EN** → **SW1 Pin 1** (reset button)
+    - **SW1 Pin 2** → **GND** (when button pressed, EN goes LOW = reset)
+  - **Note:** EN must be HIGH (3.3V) for ESP32 to operate. Pulling it LOW resets the chip.
+- **U2 GPIO0 (Boot Mode Pin):**
+  - **Function:** Boot mode selection
+  - **HIGH (3.3V):** Normal boot from flash
+  - **LOW (GND):** Download mode for flashing
+  - **Pull-up resistor:** R4 (10kΩ) → +3V3 (required by datasheet)
+  - **Boot button:** SW2 connected to GPIO0 (pull LOW for download mode)
+  - **Connection:** U2.GPIO0 → R4 → +3V3, U2.GPIO0 → SW2 Pin 1, SW2 Pin 2 → GND
+
+**GPIO Connections:**
+- **U2 GPIO17 (UART1 TX):** → Label: `ESP32_TX` → Connect to Page 3 (U3.A1) - AC communication
+- **U2 GPIO16 (UART1 RX):** → Label: `ESP32_RX` → Connect to Page 3 (U3.A2) - AC communication
+- **U2 GPIO2:** → R1 (220Ω) → LED1 Anode → LED1 Cathode → GND (WiFi status indicator)
+- **U2 GPIO4:** → R2 (220Ω) → LED2 Anode → LED2 Cathode → GND (BLE status indicator)
+- **U2 GPIO1 (UART0 TX):** → Label: `UART_TX` → Connect to Page 4 (J2 Pin 3) [if programming header]
+- **U2 GPIO3 (UART0 RX):** → Label: `UART_RX` → Connect to Page 4 (J2 Pin 4) [if programming header]
+
+**Programming Header Connections (Optional):**
+- **U2 GPIO0:** → Label: `DTR` → Connect to Page 4 (J2 Pin 5) - Auto-reset for flashing
+- **U2 EN:** → Label: `RTS` → Connect to Page 4 (J2 Pin 6) - Auto-reset for flashing
+
+**Note:** According to ESP32-WROOM-32E datasheet:
+- **Power supply:** Must be stable 3.0V to 3.6V (we use 3.3V)
+- **Peak current:** Up to 500mA during WiFi transmission
+- **Decoupling:** 100nF ceramic capacitor required at exposed VDD pin (Pin 2)
+- **Bulk capacitor:** 10µF recommended near module (C6)
+- **PCB layout:** Decoupling capacitors must be placed as close as possible to Pin 2
+- **Module variant:** Your module (onboard antenna) only exposes Pin 2 as VDD - internal VDD pins are handled by the module
+
+**Button Connections:**
+- **SW1 (Reset Button) - Connected to EN Pin (Pin 3 in RF_Module library):**
+  - **SW1 Pin 1** → **U2.EN** (Enable pin - Pin 3 in RF_Module library)
+  - **SW1 Pin 1** → **R3 (10kΩ)** → **+3V3** (pull-up resistor)
+  - **SW1 Pin 2** → **GND**
+  - **Function:** Pressing SW1 pulls EN LOW, which resets the ESP32
+  - **Normal state:** EN is HIGH (3.3V) via R3 pull-up, ESP32 operates normally
+  - **Reset state:** When button pressed, EN goes LOW (GND), ESP32 resets
+- **SW2 (Boot Button) - Connected to GPIO0:**
+  - **SW2 Pin 1** → **U2.GPIO0** (Boot mode pin)
+  - **SW2 Pin 1** → **R4 (10kΩ)** → **+3V3** (pull-up resistor)
+  - **SW2 Pin 2** → **GND**
+  - **Function:** Pressing SW2 pulls GPIO0 LOW, which puts ESP32 in download mode
+  - **Normal state:** GPIO0 is HIGH (3.3V) via R4 pull-up, ESP32 boots from flash
+  - **Download mode:** When button pressed, GPIO0 goes LOW (GND), ESP32 enters download mode
+
+**LED Connections:**
+- LED1 Anode → R1 → U2.GPIO2
+- LED1 Cathode → GND
+- LED2 Anode → R2 → U2.GPIO4
+- LED2 Cathode → GND
+
+**Decoupling Capacitors (For Module with Only Pin 2 VDD Exposed):**
+- **C5:** U2 Pin 2 (VDD) → GND (100nF ceramic, 0805 package)
+  - **Purpose:** High-frequency decoupling for VDD pin
+  - **Placement:** As close as possible to Pin 2 (<5mm)
+- **C6:** U2 Pin 2 (VDD) → GND (10µF ceramic, 0805 package)
+  - **Purpose:** Bulk capacitor for power supply stability
+  - **Placement:** Near ESP32 module, close to Pin 2
+
+**Note:** 
+- Your ESP32-WROOM-32E module (onboard antenna) only exposes Pin 2 as VDD
+- Internal VDD pins are handled internally by the module
+- Only the exposed Pin 2 requires external decoupling capacitors
+- C5 (100nF) for high-frequency decoupling
+- C6 (10µF) for bulk power supply filtering
+
+**PCB Layout Requirements:**
+- **C5 (100nF):** Place **as close as possible** to Pin 2 (<5mm recommended)
+- **C6 (10µF):** Place near ESP32 module, close to Pin 2
+- **Trace width:** Use short, wide traces from Pin 2 to capacitors
+- **Ground connection:** Connect capacitors to ground plane with short, wide traces
+- **Power trace:** Use adequate trace width for 500mA peak current (minimum 0.5mm)
+
+---
+
+### Page 3: Level Shifter and AC Interface
+
+| Ref | Component | Library | Symbol | Value | Notes |
+|-----|-----------|---------|--------|-------|-------|
+| U3 | Level Shifter | `Midea_ESP` | `TXB0104PWR` | TXB0104PWR | 4-channel level shifter (TSSOP-14) |
+| J1 | AC Connector | `Connector_JST` | `JST_XH_B4B-XH-A` | - | 4-pin JST-XH |
+| C14 | Capacitor | `Device` | `C` | 100nF | VCCA decoupling (U3 Pin 12) |
+| C15 | Capacitor | `Device` | `C` | 100nF | VCCB decoupling (U3 Pin 11) |
+
+**TXB0104PWR Pin Connections:**
+
+**Low Voltage Side (3.3V - ESP32):**
+- **U3 Pin 1 (A1)** → Net Label: `ESP32_TX` → Connect to Page 2 (U2.GPIO17)
+- **U3 Pin 2 (A2)** → Net Label: `ESP32_RX` → Connect to Page 2 (U2.GPIO16)
+- **U3 Pin 3 (A3)** → NC (Not Connected)
+- **U3 Pin 4 (A4)** → NC (Not Connected)
+
+**High Voltage Side (5V - AC):**
+- **U3 Pin 9 (B1)** → Net Label: `AC_RX` → J1 Pin 2
+- **U3 Pin 8 (B2)** → Net Label: `AC_TX` → J1 Pin 3
+- **U3 Pin 7 (B3)** → NC (Not Connected)
+- **U3 Pin 6 (B4)** → NC (Not Connected)
+
+**Power (Per TXB0104 Datasheet):**
+- **U3 Pin 12 (VCCA)** → **+3V3 Power Rail** (Low voltage side: 1.2V to 3.6V, we use 3.3V)
+  - **C14 (100nF)** → **U3 Pin 12 (VCCA)** → **+3V3**, **C14 (other terminal)** → **GND** (decoupling capacitor - required by datasheet)
+- **U3 Pin 11 (VCCB)** → **+5V Power Rail** (High voltage side: 1.65V to 5.5V, we use 5V)
+  - **C15 (100nF)** → **U3 Pin 11 (VCCB)** → **+5V**, **C15 (other terminal)** → **GND** (decoupling capacitor - required by datasheet)
+- **U3 Pin 10 (OE)** → **+3V3 Power Rail** (Output Enable - referenced to VCCA per datasheet)
+  - **Note:** OE input circuit is referenced to VCCA (not VCCB) per datasheet
+  - **Function:** HIGH (3.3V) = enabled, LOW (GND) = high-impedance state
+- **U3 Pin 5 (GND)** → GND
+- **U3 Pin 13 (GND)** → GND
+- **U3 Pin 14 (GND)** → GND
+
+**Critical Requirement (Per Datasheet):**
+- **VCCA must NOT exceed VCCB:** 3.3V ≤ 5V ✓ (correct)
+- **Decoupling capacitors:** 100nF ceramic capacitors required on both VCCA and VCCB (C14, C15)
+
+**AC Connector (J1) - JST-XH Connector on PCB:**
+- **J1 Pin 1** → **+5V Power Rail** → Connect to Page 1 (U1 Pin 3 via capacitors) - **Power input for PCB**
+- **J1 Pin 2** → Net Label: `AC_RX` → U3 Pin 9 (B1)
+- **J1 Pin 3** → Net Label: `AC_TX` → U3 Pin 8 (B2)
+- **J1 Pin 4** → **GND** → Connect to all GND nets
+
+**Note:** J1 is a JST-XH connector mounted 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)
+
+You will connect a cable with a matching JST-XH connector on one end to connect to your AC unit. The other end of the cable connects to J1 on the PCB.
+
+**Net Labels to Use:**
+- `ESP32_TX` - ESP32 transmit to level shifter
+- `ESP32_RX` - ESP32 receive from level shifter
+- `AC_TX` - AC transmit line
+- `AC_RX` - AC receive line
+
+---
+
+### Page 4: Programming Header (Required for Flashing)
+
+| Ref | Component | Library | Symbol | Value | Notes |
+|-----|-----------|---------|--------|-------|-------|
+| J2 | Header | `Connector_PinHeader_2.54mm` | `PinHeader_2x04_P2.54mm_Vertical` | - | 2x4 programming header (8 pins total, 6 used) |
+| R5 | Resistor | `Device` | `R` | 10kΩ | DTR pull-up (optional but recommended) |
+| R6 | Resistor | `Device` | `R` | 10kΩ | RTS pull-up (optional but recommended) |
+
+**Programming Header (J2) Pinout - 2x4 Header (2.54mm pitch):**
+
+**Pin Layout (Top View):**
+```
+┌─────────────┐
+│ 1  2  3  4  │  ← Top row
+│ 5  6  7  8  │  ← Bottom row
+└─────────────┘
+```
+
+| J2 Pin | Signal | ESP32 Connection | Description |
+|--------|--------|------------------|-------------|
+| 1 | +3V3 | +3V3 Power Rail | Optional - Power ESP32 from programmer |
+| 2 | GND | GND | Ground reference (required) |
+| 3 | UART_TX | U2.GPIO1 (UART0 TX) | ESP32 transmits to programmer |
+| 4 | UART_RX | U2.GPIO3 (UART0 RX) | ESP32 receives from programmer |
+| 5 | DTR | U2.GPIO0 | Data Terminal Ready (auto-reset for flashing) |
+| 6 | RTS | U2.EN | Request To Send (auto-reset for flashing) |
+| 7 | NC | - | Not connected (spare) |
+| 8 | NC | - | Not connected (spare) |
+
+**Connections:**
+- **J2 Pin 1** → **+3V3 Power Rail** (optional - for powering from programmer)
+- **J2 Pin 2** → **GND** (required)
+- **J2 Pin 3** → Net Label: `UART_TX` → Connect to Page 2 (U2.GPIO1) - ESP32 TX
+- **J2 Pin 4** → Net Label: `UART_RX` → Connect to Page 2 (U2.GPIO3) - ESP32 RX
+- **J2 Pin 5** → Net Label: `DTR` → Connect to Page 2 (U2.GPIO0) - Auto-reset
+- **J2 Pin 6** → Net Label: `RTS` → Connect to Page 2 (U2.EN) - Auto-reset
+- **J2 Pin 7** → **NC** (Not Connected - spare for future use)
+- **J2 Pin 8** → **NC** (Not Connected - spare for future use)
+
+**Flashing with 2x4 Header:**
+- **Automatic** - no buttons needed:
+  - DTR/RTS signals automatically put ESP32 in boot mode
+  - Just run `esptool` or ESPHome - it handles everything
+  - Much easier and faster
+
+**Note:** Pins 7 and 8 are spare and can be used for future expansion if needed.
+
+**Auto-Reset Circuit (Optional but Recommended):**
+- **J2 Pin 5 (DTR)** → R5 → +3V3
+- **J2 Pin 5 (DTR)** → U2.GPIO0 (Boot mode control)
+- **J2 Pin 6 (RTS)** → R6 → +3V3
+- **J2 Pin 6 (RTS)** → U2.EN (Reset control)
+
+**Note:** The pull-up resistors (R5, R6) are optional. Most USB-to-Serial adapters have built-in pull-ups, but adding them ensures reliable operation.
+
+**Net Labels:**
+- `UART_TX` - ESP32 UART TX to programmer
+- `UART_RX` - ESP32 UART RX from programmer
+- `DTR` - Data Terminal Ready (auto-reset)
+- `RTS` - Request To Send (auto-reset)
+
+**External USB-to-Serial Adapter Connections:**
+When connecting an external USB-to-Serial adapter (e.g., CP2102, CH340, FT232):
+- Adapter **VCC** → J2 Pin 1 (optional - only if you want to power ESP32 from adapter)
+- Adapter **GND** → J2 Pin 2
+- Adapter **RX** → J2 Pin 3 (UART_TX from ESP32)
+- Adapter **TX** → J2 Pin 4 (UART_RX to ESP32)
+- Adapter **DTR** → J2 Pin 5 (auto-reset)
+- Adapter **RTS** → J2 Pin 6 (auto-reset)
+
+---
+
+## How to Add Components in KiCad
+
+### Step 1: Add Components
+1. Press **`A`** (or click "Place Symbol" tool)
+2. In the symbol chooser, search for the component
+3. Click to place on schematic
+4. Press **`E`** to edit properties (set Reference, Value)
+
+### Step 2: Add Power Symbols
+1. Press **`P`** (or click "Place Power Port" tool)
+2. Select power symbol: `+3V3`, `+5V`, or `GND`
+3. Click to place
+4. All symbols with the same name are automatically connected
+
+### Step 3: Add Wires
+1. Press **`W`** (or click "Place Wire" tool)
+2. Click on a pin, then click on destination pin
+3. KiCad will route the wire automatically
+
+### Step 4: Add Net Labels (for cross-page connections)
+1. Press **`L`** (or click "Place Net Label" tool)
+2. Type the net name (e.g., `ESP32_TX`)
+3. Click on the wire to attach the label
+4. Use the same label name on other pages to connect them
+
+### Step 5: Add Hierarchical Sheets (for multiple pages)
+1. Press **`S`** (or click "Place Hierarchical Sheet" tool)
+2. Draw a rectangle for the sheet
+3. Double-click to edit sheet properties
+4. Set sheet name and file name
+
+---
+
+## Connection Summary by Net
+
+### +3V3 Net (3.3V Power Rail)
+- U1 Pin 2 (OUT)
+- U2 All VDD pins (1, 3, 14, 21, 22, 27, 28, 33, 42)
+- U3 Pin 12 (VCCA)
+- U3 Pin 10 (OE)
+- J2 Pin 1 (optional - if powering from programmer)
+- R1, R2, R3, R4, R5, R6 (one end of pull-up resistors)
+- LED1, LED2 anodes (via resistors)
+
+### +5V Net (5V Power Rail)
+- J1 Pin 1 (Power input from AC connection)
+- U1 Pin 3 (IN)
+- U3 Pin 11 (VCCB)
+
+### GND Net (Ground)
+- J1 Pin 4 (Ground from AC connection)
+- U1 Pin 1 and TAB
+- U2 All GND pins (2, 4, 13, 15, 20, 23, 26, 29, 34, 38, 40)
+- U3 Pins 5, 13, 14 (GND)
+- J2 Pin 2 (GND)
+- All capacitor negative terminals
+- SW1 Pin 2, SW2 Pin 2
+- LED1, LED2 cathodes
+
+### ESP32_TX Net
+- U2 GPIO17 → U3 Pin 1 (A1)
+
+### ESP32_RX Net
+- U2 GPIO16 → U3 Pin 2 (A2)
+
+### AC_TX Net
+- U3 Pin 8 (B2) → J1 Pin 3
+
+### AC_RX Net
+- U3 Pin 9 (B1) → J1 Pin 2
+
+### UART_TX Net (if programming header included)
+- U2 GPIO1 → J2 Pin 3
+
+### UART_RX Net (if programming header included)
+- U2 GPIO3 → J2 Pin 4
+
+### DTR Net (if programming header included)
+- J2 Pin 5 → U2 GPIO0
+
+### RTS Net (if programming header included)
+- J2 Pin 6 → U2 EN
+
+---
+
+## Recommended Schematic Layout
+
+### Option 1: Single Page (Simple)
+- Left: Power supply (powered from J1)
+- Center: ESP32 with peripherals
+- Right: Level shifter and AC connector (J1 provides power)
+- Bottom: Programming Header (if included)
+
+### Option 2: Multiple Pages (Organized)
+- **Page 1**: Power Supply (USB input, regulator, capacitors)
+- **Page 2**: ESP32 Main (MCU, buttons, LEDs, decoupling caps)
+- **Page 3**: Level Shifter & AC Interface
+- **Page 4**: Programming Header (optional)
+
+Use hierarchical sheets or net labels to connect between pages.
+
+---
+
+## Tips
+
+1. **Use Net Labels** for cross-page connections instead of wires
+2. **Group related components** together
+3. **Place power symbols** near components that need them
+4. **Use buses** if you have multiple similar signals (not needed here)
+5. **Add text notes** to document special connections
+6. **Run ERC** (Electrical Rules Check) after completing: Tools → Electrical Rules Checker
+
+---
+
+## Component Values Summary
+
+| Component | Value | Purpose |
+|-----------|-------|---------|
+| U1 | AMS1117-3.3 | 5V to 3.3V regulator |
+| U2 | ESP32-WROOM-32E | Main microcontroller |
+| U3 | TXB0104PWR | 3.3V ↔ 5V level shifter |
+| J2 | 6-pin Header | Programming header (optional) |
+| R1, R2 | 220Ω | LED current limiting |
+| R3, R4 | 10kΩ | Button pull-up resistors |
+| R5, R6 | 10kΩ | DTR/RTS pull-up resistors (optional) |
+| C1, C2 | 10µF | Power supply capacitors |
+| C3, C4 | 100nF | Decoupling capacitors |
+| C5-C13 | 100nF | ESP32 decoupling |
+| C14, C15 | 100nF, 10µF | CP2102N decoupling |
+
+---
+
+## Next Steps After Schematic
+
+1. **Annotate Components**: Tools → Annotate Schematic
+2. **Electrical Rules Check**: Tools → Electrical Rules Checker
+3. **Assign Footprints**: Tools → Assign Footprints
+4. **Generate Netlist**: Tools → Generate Netlist
+5. **Open PCB Editor**: Click "Open PCB in Board Editor"
+