Kicad Schematic

• Rotation 0: schematic position = (sx + px, sy - py)
• Rotation 90: schematic position = (sx + py, sy + px)
• Rotation 180: schematic position = (sx - px, sy + py)
• Rotation 270: schematic position = (sx - py, sy - px)

Always use pin_abs() from the helper library — never compute these by hand.

Architecture

User describes circuit
        |
Read symbol libraries (.kicad_sym) to get pin positions
        |
Build pin position dictionaries for every multi-pin IC
        |
Write Python script using SchematicBuilder (from helper library)
  - Use connect_pin() for IC pins (computes positions automatically)
  - Use place_2pin_vertical() for passives (knows pin 1/2 positions)
        |
Generate .kicad_sch file
        |
Post-process with fix_subsymbol_names()
        |
Run ERC validation: kicad-cli sch erc --format json
        |
Parse errors -> fix script -> regenerate -> repeat (max 5 iterations)

Step-by-step Workflow

0. Ensure kicad-cli is Available

Before running any ERC validation, verify that kicad-cli is on the system PATH. Run:

which kicad-cli 2>/dev/null || where kicad-cli 2>/dev/null

If not found, check for a local KiCad installation and offer to create a symlink:

macOS:

# Check if KiCad is installed as an app
KICAD_CLI="/Applications/KiCad/KiCad.app/Contents/MacOS/kicad-cli"
if [ -f "$KICAD_CLI" ]; then
    echo "Found kicad-cli inside KiCad.app. Creating symlink..."
    sudo ln -sf "$KICAD_CLI" /usr/local/bin/kicad-cli
    echo "Done! kicad-cli is now available on PATH."
else
    echo "KiCad not found. Install from https://www.kicad.org/download/macos/"
fi

Linux:

# kicad-cli is typically installed alongside KiCad via package manager
# Check common locations
for p in /usr/bin/kicad-cli /usr/local/bin/kicad-cli /snap/kicad/current/bin/kicad-cli; do
    if [ -f "$p" ]; then
        echo "Found kicad-cli at $p"
        # If not on PATH, symlink it
        if ! command -v kicad-cli &>/dev/null; then
            sudo ln -sf "$p" /usr/local/bin/kicad-cli
        fi
        break
    fi
done
# If still not found:
# Ubuntu/Debian: sudo apt install kicad
# Fedora: sudo dnf install kicad
# Arch: sudo pacman -S kicad
# Or install from https://www.kicad.org/download/linux/

Windows:

# Check standard install path
$kicadCli = "C:\Program Files\KiCad\8.0\bin\kicad-cli.exe"
if (Test-Path $kicadCli) {
    Write-Host "Found kicad-cli. Add to PATH:"
    Write-Host '  [Environment]::SetEnvironmentVariable("PATH", $env:PATH + ";C:\Program Files\KiCad\8.0\bin", "User")'
} else {
    Write-Host "KiCad not found. Install from https://www.kicad.org/download/windows/"
}

Tell the user what you found and ask for confirmation before creating any symlinks. If kicad-cli is truly not installed, provide the download link for their OS and stop — ERC validation requires it.

1. Understand the Circuit

Before writing any code, gather:

• Component list with specific part numbers
• Power architecture (voltage rails, regulators)
• Signal connections (which pins connect to which)
• Symbol libraries needed (standard KiCad libs + any custom .kicad_sym files)

2. Read Symbol Libraries (NON-NEGOTIABLE)

For every IC and multi-pin component, read its .kicad_sym definition to get exact pin names, numbers, positions, and types. You cannot connect pins correctly without this data.

from kicad_sch_helpers import SymbolLibrary

lib = SymbolLibrary()
lib.load_from_kicad_sym("path/to/library.kicad_sym")

# Now you know exact pin positions
ad9363 = lib.get("AD9363ABCZ")
for pin in ad9363.pins:
    print(f"{pin.name} ({pin.number}): at ({pin.x}, {pin.y}), type={pin.pin_type}")

For manual/inline approaches, build a pin dictionary from the library:

# Extract from .kicad_sym file — these are LIBRARY coordinates (Y-up)
AD_PINS = {
    'TX1A_P': (-17.78, 25.40),
    'TX1A_N': (-17.78, 22.86),
    'SPI_CLK': (-17.78, -10.16),
    # ... all pins
}

# SOT-23-5 packages (common for LDOs like AP2112K, ME6211):
SOT5_PINS = {
    'VIN':  (-7.62,  2.54),   # Pin 1 - top left
    'GND':  ( 0.00, -7.62),   # Pin 2 - bottom center
    'EN':   (-7.62, -2.54),   # Pin 3 - bottom left
    'NC':   ( 7.62, -2.54),   # Pin 4 - bottom right  <- NOT VOUT!
    'VOUT': ( 7.62,  2.54),   # Pin 5 - top right     <- THIS is VOUT!
}

WARNING — SOT-23-5 pin trap: VOUT is at (7.62, +2.54) and NC is at (7.62, -2.54). These are only 5.08mm apart. Confusing them means your LDO output goes nowhere. Always verify from the actual library file.

3. Write the Generator Script

Use SchematicBuilder for all schematic construction. The key method is connect_pin() which computes exact pin positions automatically:

from kicad_sch_helpers import SchematicBuilder, SymbolLibrary, snap

lib = SymbolLibrary()
lib.load_from_kicad_sym("custom_symbols.kicad_sym")

sch = SchematicBuilder(symbol_lib=lib, project_name="my_project")
sch.set_lib_symbols(lib_symbols_content)  # Raw S-expression for embedded symbols

# Place an IC
sch.place("CubeSat_SDR:AD9363ABCZ", "U1", "AD9363ABCZ",
          x=320, y=200, footprint="CubeSat_SDR:AD9363_BGA144")

# Connect pins by NAME — coordinates computed automatically
sch.connect_pin("U1", "TX1A_P", "TX1A_P", wire_dx=-5.08)
sch.connect_pin("U1", "SPI_CLK", "SPI_CLK", wire_dy=-5.08)
sch.connect_pin("U1", "GND", "GND", wire_dy=5.08)

# For unused pins, add no-connect flags
sch.connect_pin_noconnect("U1", "AUXDAC1")

# For 2-pin passives, use convenience helpers
from kicad_sch_helpers import place_2pin_vertical
place_2pin_vertical(sch, "Device:C", "C1", "100nF",
                    x=snap(230), y=snap(155),
                    top_net="VCC_3V3", bottom_net="GND",
                    footprint="Capacitor_SMD:C_0402_1005Metric")

If using inline pin dictionaries (without SymbolLibrary), use pin_abs():

from kicad_sch_helpers import pin_abs, snap

GRID = 1.27

def wl(sch, sx, sy, pin_name, pins_dict, net, dx=0, dy=0, rot=0, label_angle=0):
    """Wire + Label: connect an IC pin to a net label."""
    px, py = pin_abs(sx, sy, pins_dict[pin_name][0], pins_dict[pin_name][1], rot)
    ex, ey = snap(px + dx), snap(py + dy)
    if dx != 0 or dy != 0:
        sch.w(px, py, ex, ey)
    sch.label(net, ex, ey, label_angle)

# Usage:
wl(sch, 320, 200, 'TX1A_P', AD_PINS, "TX1A_P", dx=-7.62)

4. Handle the lib_symbols Section

Every symbol referenced must be embedded in the schematic's lib_symbols. Three critical rules:

1. Parent symbols use the full lib_id: (symbol "Device:R" ...)
2. Sub-symbols must NOT have the library prefix: (symbol "R_0_1" ...) not (symbol "Device:R_0_1" ...)
3. Always post-process with fix_subsymbol_names() to catch any mistakes

Use fix_subsymbol_names() as a post-processing step:

from kicad_sch_helpers import fix_subsymbol_names

content = sch.build(title="My Schematic")
content = fix_subsymbol_names(content)

The regex-based fixer handles nested sub-symbols at any depth and any library prefix format.

5. Grid Snapping (Prevents 90% of Warnings)

Every coordinate in the schematic must be a multiple of 1.27mm. Use snap():

from kicad_sch_helpers import snap

# snap() rounds to nearest 1.27mm grid point
x = snap(123.45)  # -> 124.46 (nearest multiple of 1.27)

Apply snap() to: component positions, wire endpoints, label positions, no-connect positions, and PWR_FLAG positions. The connect_pin() and pin_abs() functions do this automatically.

6. Add PWR_FLAG Symbols

For every power net that originates from a voltage regulator (not a power symbol), add a PWR_FLAG to prevent "power_pin_not_driven" errors:

# Define PWR_FLAG in lib_symbols (see references/kicad_sexpression_format.md)
# Then place on each power net:
sch.place_pwr_flag(x=70, y=78, net_name="VCC_3V3A")

Rule of thumb: If a net is driven by a component whose output pin type is passive (not power_out), that net needs a PWR_FLAG. This includes most LDO regulators.

Also place PWR_FLAG on GND nets that don't have a dedicated GND power symbol driving them.

7. No-Connect Flags

Every unused pin on every IC MUST have a no-connect flag. Missing no-connect flags cause pin_not_connected errors.

# Using SchematicBuilder:
sch.connect_pin_noconnect("U1", "AUXDAC1")

# Or manually with pin_abs:
px, py = pin_abs(sx, sy, pin_x, pin_y, rotation)
sch.nc(px, py)

8. Validate with kicad-cli

from kicad_sch_helpers import run_erc

result = run_erc("output/schematic.kicad_sch")
print(f"Errors: {result['errors']}, Warnings: {result['warnings']}")

if result['errors'] > 0:
    for detail in result['details']:
        if detail.get('severity') == 'error':
            print(f"  {detail['type']}: {detail.get('description', '')}")

9. Automated Fix Loop

For complex schematics, use the validation loop:

from kicad_sch_helpers import validate_and_fix_loop

def my_fixer(erc_result, iteration):
    """Analyze ERC errors and apply fixes. Return True if fixes applied."""
    error_types = erc_result.get('error_types', {})

    if 'pin_not_connected' in error_types:
        # Read the schematic, find unconnected pins, add connections
        # ... fix logic ...
        return True

    if 'label_dangling' in error_types:
        # Move labels to correct pin positions
        # ... fix logic ...
        return True

    return False  # No fixable errors found

final = validate_and_fix_loop("output/schematic.kicad_sch", my_fixer)

Fixing ERC on Existing Schematics

When the user has an existing .kicad_sch with ERC errors (not generating a new schematic), use this workflow.

Step 1: Run ERC with JSON Output

Always use --format json -o file.json --severity-all. Never pipe kicad-cli output to stdout — it writes JSON to the file specified by -o.

On macOS, kicad-cli needs environment variables to find the standard libraries:

KICAD9_SYMBOL_DIR="/Applications/KiCad/KiCad.app/Contents/SharedSupport/symbols" \
KICAD9_FOOTPRINT_DIR="/Applications/KiCad/KiCad.app/Contents/SharedSupport/footprints" \
/Applications/KiCad/KiCad.app/Contents/MacOS/kicad-cli sch erc \
  --format json --severity-all -o /tmp/erc_result.json schematic.kicad_sch

Or use the helper:

from kicad_sch_helpers import run_erc
result = run_erc("schematic.kicad_sch", env_vars={
    "KICAD9_SYMBOL_DIR": "/Applications/KiCad/KiCad.app/Contents/SharedSupport/symbols",
    "KICAD9_FOOTPRINT_DIR": "/Applications/KiCad/KiCad.app/Contents/SharedSupport/footprints",
})

Step 2: Parse and Categorize Violations

import json
with open("/tmp/erc_result.json") as f:
    report = json.load(f)

violations = []
for sheet in report.get("sheets", []):
    violations.extend(sheet.get("violations", []))

# Categorize by severity and type
errors = [v for v in violations if v.get("severity") == "error"]
warnings = [v for v in violations if v.get("severity") == "warning"]
by_type = {}
for v in violations:
    t = v.get("type", "unknown")
    by_type.setdefault(t, []).append(v)

print(f"Errors: {len(errors)}, Warnings: {len(warnings)}")
for t, items in sorted(by_type.items()):
    print(f"  {t}: {len(items)}")

Note: The JSON format nests violations under sheets[].violations[], not at the top level.

Step 3: Write Targeted Python Fix Scripts

Never manually edit .kicad_sch files — always write Python scripts. The s-expression format is sensitive to whitespace and parenthesis balance.

Key utility functions (all in scripts/kicad_sch_helpers.py):

from kicad_sch_helpers import (
    find_block,                    # Find balanced parenthesized block
    remove_block_with_whitespace,  # Clean removal preserving formatting
    extract_embedded_symbol,       # Extract from lib_symbols section
    convert_embedded_to_library,   # Embedded → standalone library format
    find_by_uuid,                  # Locate element by UUID
    remove_by_uuid,                # Remove element by UUID
    replace_lib_id,                # Bulk lib_id replacement
    replace_footprint,             # Bulk footprint replacement
    fix_annotation_suffixes,       # Add numeric suffixes to bare refs
    create_pwr_flag_block,         # Generate PWR_FLAG s-expression
)

Step 4: Common Fix Patterns

Remove a symbol by UUID:

content = remove_by_uuid(content, "uuid-string", "symbol")

Replace a lib_id across all instances:

content = replace_lib_id(content, "Connector:Conn_01x04", "CubeSat_SDR:Conn_01x04")

Add PWR_FLAG to fix power_pin_not_driven:

pwr_block = create_pwr_flag_block(
    x=34.29, y=77.47, ref_num=7,
    project_name="my_project",
    root_uuid="5fb33c66-7637-43ae-9eef-34b4f23f6cfb"
)
# Insert before the final closing paren
last_close = content.rstrip().rfind(')')
content = content[:last_close] + '\n' + pwr_block + '\n' + content[last_close:]

Suppress warnings in .kicad_pro:

import json
with open("project.kicad_pro") as f:
    pro = json.load(f)
pro["erc"]["rule_severities"]["lib_symbol_mismatch"] = "ignore"
with open("project.kicad_pro", "w") as f:
    json.dump(pro, f, indent=2)
    f.write('\n')

Step 5: Iterative Fix-Verify Loop

Always run ERC after each batch of fixes. Some fixes expose new issues:

1. Run ERC → parse results → categorize
2. Fix the highest-priority errors first (see error priority in references)
3. Run ERC again → verify error count dropped
4. Repeat until 0 errors (warnings may be suppressed if justified)

Back up the schematic before running fix scripts. Use shutil.copy2().

KiCad 8→9 Migration

When validating a KiCad 8 schematic with KiCad 9, expect these categories of issues:

Symbol Renames (lib_symbol_issues)

Fix strategy: Create a project-level custom library with KiCad 8 symbol versions. Change lib_ids to point to the custom library. Do NOT try to update to KiCad 9 versions — pin positions differ and will break wire connections.

Pin Position Changes (lib_symbol_mismatch)

CRITICAL: Do NOT replace embedded Device:C/R/L symbols with KiCad 9 versions.

KiCad 9 changed passive pin positions:

• KiCad 8: Device:C pins at (0, ±2.54)
• KiCad 9: Device:C pins at (0, ±3.81)

Replacing embedded symbols breaks every wire connected to every capacitor, resistor, and inductor. Instead, suppress lib_symbol_mismatch in .kicad_pro — the embedded KiCad 8 symbols work fine.

Footprint Renames (footprint_link_issues)

Use replace_footprint() for bulk updates.

Annotation Requirements

KiCad 9 requires all reference designators to end with a digit. References like C_RX1B_N or J_PWR will cause "Item not annotated" errors in the GUI (but NOT in CLI ERC).

from kicad_sch_helpers import fix_annotation_suffixes
content = fix_annotation_suffixes(content)  # Adds "1" suffix to bare refs

Migration Workflow

1. Run ERC → categorize violations
2. Create custom library with KiCad 8 symbol versions (extract from embedded lib_symbols)
3. Update lib_ids from standard libraries to custom library
4. Update renamed footprints
5. Fix annotation suffixes
6. Add PWR_FLAG for any new power_pin_not_driven errors
7. Suppress lib_symbol_mismatch in .kicad_pro (safe — embedded symbols still work)
8. Suppress multiple_net_names if intentional dual-naming exists
9. Run ERC again → verify 0 errors

Custom Library Management

When standard KiCad libraries change between versions, create project-level libraries to preserve compatibility.

Creating Project Library Tables

sym-lib-table (in project root):

(sym_lib_table
  (version 7)
  (lib (name "CubeSat_SDR")(type "KiCad")(uri "${KIPRJMOD}/libraries/cubesat_sdr.kicad_sym")(options "")(descr "Project custom symbols"))
)

fp-lib-table (in project root):

(fp_lib_table
  (version 7)
  (lib (name "CubeSat_SDR")(type "KiCad")(uri "${KIPRJMOD}/libraries/cubesat_sdr.pretty")(options "")(descr "Project custom footprints"))
)

Use ${KIPRJMOD} for portable paths — it resolves to the project directory.

Extracting Embedded Symbols to Library

When migrating from standard library symbols to custom ones:

from kicad_sch_helpers import extract_embedded_symbol, convert_embedded_to_library

# Read schematic
with open("schematic.kicad_sch") as f:
    sch = f.read()

# Extract a symbol from the embedded lib_symbols section
block = extract_embedded_symbol(sch, "Connector:Conn_01x04")

# Convert from embedded format (prefix:Name) to library format (Name)
lib_block = convert_embedded_to_library(block, "Connector", "Conn_01x04")

# Append to custom library file (before the final closing paren)
with open("libraries/custom.kicad_sym") as f:
    lib = f.read()
close_pos = lib.rstrip().rfind(')')
lib = lib[:close_pos] + '\t' + lib_block + '\n' + lib[close_pos:]
with open("libraries/custom.kicad_sym", "w") as f:
    f.write(lib)

Embedded vs Library Format

In .kicad_sch embedded lib_symbols: top-level is (symbol "Library:Name" ...), sub-symbols use (symbol "Name_0_1" ...).

In .kicad_sym library files: top-level is (symbol "Name" ...), sub-symbols use (symbol "Name_0_1" ...).

The only difference is the top-level name loses its library prefix.

Common Patterns

Decoupling Capacitor Array

for i, (ref, val) in enumerate(zip(refs, values)):
    place_2pin_vertical(sch, "Device:C", ref, val,
                        x=snap(start_x + i * 8), y=snap(cap_y),
                        top_net=power_net, bottom_net="GND",
                        footprint=f"Capacitor_SMD:{fp}")

2-Pin Passives (R, C, L)

Standard KiCad 2-pin passive symbols have:

• Pin 1 at library (0, 2.54) — top when vertical
• Pin 2 at library (0, -2.54) — bottom when vertical

With rotation 0 at schematic (sx, sy):

• Pin 1 schematic position: (sx, sy - 2.54)
• Pin 2 schematic position: (sx, sy + 2.54)

place_2pin_vertical(sch, "Device:C", "C1", "100nF",
                    x=snap(100), y=snap(150),
                    top_net="VCC_3V3", bottom_net="GND",
                    footprint="Capacitor_SMD:C_0402_1005Metric")

Multi-pin IC Connection

# Always use connect_pin — never compute positions manually
signal_map = {
    "TX1A_P": "TX1A_P",
    "TX1A_N": "TX1A_N",
    "SPI_CLK": "SPI_CLK",
    # ... all signal pins
}
for pin_name, net_name in signal_map.items():
    sch.connect_pin("U1", pin_name, net_name, wire_dx=-7.62)

# Power pins
for pin_name in ["VDDD1P3", "VDDA1P3", "VDDD1P8"]:
    sch.connect_pin("U1", pin_name, f"VCC_{pin_name}", wire_dy=5.08)

# Unused pins — EVERY unused pin needs this
for pin_name in ["AUXDAC1", "AUXDAC2", "AUXADC", "TEMP_SENS"]:
    sch.connect_pin_noconnect("U1", pin_name)

Power Regulator with PWR_FLAG

sch.place("CubeSat_SDR:AP2112K", "U4", "AP2112K-3.3",
          x=snap(100), y=snap(180),
          footprint="Package_TO_SOT_SMD:SOT-23-5")
wl(sch, 100, 180, 'VIN',  SOT5_PINS, "VCC_5V",  dx=-7.62)
wl(sch, 100, 180, 'EN',   SOT5_PINS, "VCC_5V",  dx=-7.62)
wl(sch, 100, 180, 'GND',  SOT5_PINS, "GND",     dy=5.08)
wl(sch, 100, 180, 'VOUT', SOT5_PINS, "VCC_3V3", dx=7.62)
# NC pin — no-connect flag, NOT a label
nc_x, nc_y = pin_abs(100, 180, *SOT5_PINS['NC'])
sch.nc(nc_x, nc_y)
# PWR_FLAG on output net
sch.place_pwr_flag(x=snap(115), y=snap(178), net_name="VCC_3V3")

Lessons Learned (Battle-Tested)

These lessons came from debugging a real 119-component CubeSat SDR schematic:

1. Never guess pin positions. Even being off by 1.27mm (one grid unit) causes ERC errors. Always read the .kicad_sym file and use computed positions.

2. The Y-axis flip is the #1 source of bugs. Library Y-up vs schematic Y-down means you must negate Y. A pin at library (0, 25.4) is at schematic (sx, sy - 25.4) — NOT (sx, sy + 25.4). Getting this wrong places labels 50mm from their pins.

3. SOT-23-5 VOUT vs NC confusion silently breaks LDO circuits. VOUT=(7.62, 2.54), NC=(7.62, -2.54). They differ only in Y sign. After the Y-flip, VOUT is above NC in the schematic. Always verify against the library.

4. Sub-symbol naming breaks KiCad silently. If you write (symbol "Device:R_0_1" ...) instead of (symbol "R_0_1" ...), KiCad may open the file but all symbols appear broken. Always run fix_subsymbol_names().

5. PWR_FLAG is needed more often than you think. Any net driven by a regulator with passive-type output pins needs one. Also add one on GND. Missing PWR_FLAGs cause power_pin_not_driven errors on every component on that net.

6. Grid snapping prevents hundreds of warnings. A single off-grid component cascades into off-grid warnings for all connected wires and labels. Snap everything from the start.

7. Account for every pin. Go through the pin list systematically. Every pin must be either: connected via wire+label, connected to a power symbol, or flagged with no_connect. Missing even one pin produces an error.

8. Parenthesis balance check. KiCad S-expressions must have perfectly balanced parentheses. Add a check at the end of generation:

   depth = sum(1 if c == '(' else -1 if c == ')' else 0 for c in content)
   assert depth == 0, f"Parenthesis imbalance: depth={depth}"
   

9. Don't replace embedded Device:C/R/L with KiCad 9 versions. KiCad 9 changed passive pin positions from ±2.54 to ±3.81. Replacing embedded symbols breaks every wire connection. Suppress lib_symbol_mismatch instead.

10. kicad-cli JSON goes to file, not stdout. Always use -o /tmp/result.json. Piping to python gives empty stdin. The JSON is nested under sheets[].violations[], not at the top level.

11. CLI ERC doesn't check annotations. The GUI flags "Item not annotated" for references not ending with a digit (e.g., C_RX1B_N), but CLI ERC silently passes. Always run fix_annotation_suffixes() when migrating.

12. macOS kicad-cli needs environment variables. Without KICAD9_SYMBOL_DIR and KICAD9_FOOTPRINT_DIR, kicad-cli can't find the global libraries and produces false lib_symbol_issues warnings.

13. Don't use grep -P on macOS. PCRE mode is not supported. Use Python regex for all pattern matching on schematic files.

14. Create project-level library tables for custom symbols. Use ${KIPRJMOD} for portable paths. Extract embedded symbols to populate the library — don't rewrite them from scratch.

15. Back up before running fix scripts. A broken parenthesis balance renders the schematic unloadable. Use shutil.copy2() before any modifications.

16. Don't suppress ERC errors, only warnings. Suppressing lib_symbol_mismatch (warnings) is safe for KiCad 8→9 migration. Never suppress actual errors like pin_not_connected or power_pin_not_driven.

Reference Files

• scripts/kicad_sch_helpers.py — Python helper library (always use this)
• references/kicad_sexpression_format.md — KiCad S-expression format specification, coordinate system, common ERC errors and fixes

Read references/kicad_sexpression_format.md before generating any schematic to understand the coordinate system, sub-symbol naming rules, and PWR_FLAG requirements.

Checklist Before Delivery

New Schematic Generation

1. All coordinates snapped to 1.27mm grid via snap()
2. Every IC pin either connected via connect_pin() / wl() or flagged with connect_pin_noconnect() / nc()
3. Sub-symbol names fixed with fix_subsymbol_names()
4. PWR_FLAG on every voltage regulator output net AND on GND
5. ERC validation run (0 errors target, warnings acceptable)
6. Parenthesis balance verified (depth 0 at end of file)
7. Pin positions verified against .kicad_sym library (not guessed)
8. SOT-23-5 VOUT vs NC positions double-checked for all LDOs

Existing Schematic Fixing / KiCad 9 Migration

9. All reference designators end with a digit (fix_annotation_suffixes())
10. Renamed/missing symbols handled via project-level custom library
11. Embedded Device:C/R/L symbols NOT replaced (suppress lib_symbol_mismatch instead)
12. Renamed footprints updated (replace_footprint())
13. PWR_FLAG added on all power input nets including external power (barrel jack, USB VBUS)
14. Schematic backed up before running any fix scripts
15. Environment variables set for kicad-cli on macOS (KICAD9_SYMBOL_DIR, KICAD9_FOOTPRINT_DIR)
16. ERC run with --severity-all to catch all warning types