# paste_stencil.tcl — FlatCAM beta 8.995
# Automates B.Paste Gerber -> G-code for stencil milling
# Tool: 0.5mm flat end mill (corn bit)
#
# Usage (headless):
#   python flatcam.py --shellfile=paste_stencil.tcl --headless=1

# ─── USER CONFIGURATION ───────────────────────────────────────────────────────

set GERBER   "gerbers/myboard-B_Paste.gbp"   ;# path to your B.Paste Gerber
set OUTPUT   "gcode/stencil.nc"              ;# output G-code file

# Tool
set TOOL_DIA   0.5       ;# mm — 0.5mm corn bit

# Stencil material depth
# Brass shim 0.15mm → use -0.18, polyimide 0.1mm → use -0.13
set CUT_Z      -0.2      ;# mm — cutting depth (negative)
set TRAVEL_Z    2.0      ;# mm — safe travel height

# Feeds & speeds
set FEEDRATE   300       ;# mm/min
set SPINDLE  24000       ;# RPM

# NCC (copper_clear) settings
# overlap is in PERCENT (0–100), not fraction — 8.995 change from classic
set OVERLAP    60        ;# % — 60% overlap for clean clearing with 0.5mm tool
set MARGIN     0.0       ;# mm — 0 = clear exactly to aperture edge

# Multidepth — set dpp to 0 to disable (single pass)
set DPP        0.0       ;# mm per pass; 0 = single full-depth pass

# ─── DERIVED NAMES ────────────────────────────────────────────────────────────

set GBR_NAME  "paste_gerber"
set NCC_GEO   "paste_paint_geo"
set CNC_JOB   "paste_cnc"

# ─── SCRIPT ───────────────────────────────────────────────────────────────────

# 1. Fresh project
new

# 2. Load B.Paste Gerber
open_gerber $GERBER -outname $GBR_NAME

# 3. Paint (pocket) each aperture opening
#    -all processes every polygon in the object
#    method lines is most reliable for small SMD apertures
paint $GBR_NAME \
    -tooldia  $TOOL_DIA \
    -overlap  $OVERLAP  \
    -offset   $MARGIN   \
    -method   lines     \
    -connect  1         \
    -contour  1         \
    -all               \
    -outname  $NCC_GEO

# 4. Generate CNC job
#    -dpp 0 means single pass (multidepth disabled)
#    -pp default uses the standard grbl-compatible preprocessor
cncjob $NCC_GEO \
    -dia          $TOOL_DIA  \
    -z_cut        $CUT_Z     \
    -z_move       $TRAVEL_Z  \
    -feedrate     $FEEDRATE  \
    -spindlespeed $SPINDLE   \
    -pp           GRBL_11    \
    -outname      $CNC_JOB

# 5. Write G-code to file
write_gcode $CNC_JOB $OUTPUT

puts "Done: $OUTPUT"

# Clear project so FlatCAM doesn't prompt to save on exit
new
quit_app