kicad/scripting/plugins/OutputGeneration/FabOutputs.py

186 lines
6.6 KiB
Python

import pcbnew
import os
from datetime import datetime
from pathlib import Path
__all__ = ["FabOutputs"]
class FabOutputs(pcbnew.ActionPlugin):
def defaults(self):
self.name = "Generate Outputs"
self.category = "Output Generation"
self.description = "Generate Gerbers, BOM, Drawings, etc and add to pdf/zip"
self.pcbnew_icon_support = hasattr(self, "show_toolbar_button")
self.show_toolbar_button = True
def Run(self):
# ================
# General Data
# ================
now = datetime.now()
pcb = pcbnew.GetBoard()
path_cwd = Path.cwd()
path_pcb = Path(pcb.GetFileName())
dir_pcb = path_pcb.parent
dir_fab = dir_pcb / "FabricationOutputs"
dir_asy = dir_pcb / "AssemblyOutputs"
project_name = path_pcb.stem
part_number = pcb.GetTitleBlock().GetTitle()
rev = str.upper(pcb.GetTitleBlock().GetRevision())
suffix = ""
suffix += f"_REV{rev}"
suffix += f"_{now.strftime('%Y%m%d_%H%M%S')}"
layer_count = pcb.GetDesignSettings().GetCopperLayerCount()
layer_info = [
("Front Paste", "gtp", pcbnew.F_Paste),
("Front Silkscreen", "gto", pcbnew.F_SilkS),
("Front Mask", "gts", pcbnew.F_Mask),
("Front Copper", "gtl", pcbnew.F_Cu),
*[(f'Inner Layer {layer} Copper', f'g{layer}', layer) for layer in range(1, layer_count-1)],
('Back Copper', 'gbl', pcbnew.B_Cu),
('Back Mask', 'gbs', pcbnew.B_Mask),
('Back SilkScreen', 'gbo', pcbnew.B_SilkS),
('Back Paste', 'gbp', pcbnew.B_Paste),
('Edges Cuts', 'gm1', pcbnew.Edge_Cuts),
('Drill', 'drl', None),
]
stackup = [
# [pcbnew layer, file extension, thickness, comment]
[pcbnew.F_Paste, 'gtp', None, "SN63/PB37"],
[pcbnew.F_SilkS, 'gto', None, "White"],
[pcbnew.F_Mask, 'gts', 1, "Explicit mask material"],
[None, None, None, "ENIG"],
[pcbnew.F_Cu, 'gtl', 2.1, "copper roughness"],
[None, None, 10, "Dielectric stuff"],
[1, 'g1', 0.7, "Copper roughness"],
[None, None, 24, "Dielectric stuff"],
[None, None, 12, "Dielectric stuff"],
[2, 'g2', 0.7, "Copper roughness"],
[None, None, 10, "Dielectric stuff"],
[pcbnew.B_Cu, 'gbl', 2.1, "copper roughness"],
[None, None, None, "ENIG"],
[pcbnew.B_Mask, 'gbs', 1, "Explicit mask material"],
[pcbnew.B_SilkS, 'gbo', None, "White"],
[pcbnew.B_Paste, 'gbp', None, "SN63/PB37"],
]
board_features = {
"core cap": True,
"castellated": False,
"plated board edge": False,
"copper finish": "ENIG",
"hard gold": False,
"bevelled edge": False,
"soldermask defined": None, # TODO: how do I want to determine this?
}
# ================
# Gerbers
# ================
plot_controller = pcbnew.PLOT_CONTROLLER(pcb)
plot_options = plot_controller.GetPlotOptions()
# Set General Options:
plot_options.SetOutputDirectory(dir_fab)
plot_options.SetPlotFrameRef(False)
plot_options.SetPlotValue(False)
plot_options.SetPlotReference(True)
plot_options.SetPlotInvisibleText(False)
plot_options.SetPlotViaOnMaskLayer(False)
plot_options.SetExcludeEdgeLayer(True)
plot_options.SetUseAuxOrigin(False)
plot_options.SetMirror(False)
plot_options.SetNegative(False)
#plot_options.SetDrillMarksType(PLOT_DRILL_MARKS_TYPE)
#plot_options.SetScale(PLOT_SCALE)
plot_options.SetAutoScale(True)
#plot_options.SetPlotMode(PLOT_MODE)
#plot_options.SetLineWidth(pcbnew.FromMM(PLOT_LINE_WIDTH))
plot_options.SetUseGerberAttributes(True)
plot_options.SetUseGerberProtelExtensions(False)
plot_options.SetCreateGerberJobFile(False)
plot_options.SetSubtractMaskFromSilk(True)
plot_options.SetIncludeGerberNetlistInfo(False)
plot_plan = [
# ( layer ID, file extension, description)
( pcbnew.F_Paste, 'gtp', 'Front Paste' ),
( pcbnew.F_SilkS, 'gto', 'Front SilkScreen' ),
( pcbnew.F_Mask, 'gts', 'Front Mask' ),
( pcbnew.F_Cu, 'gtl', 'Front Copper' ),
*[(layer, f'g{layer}', f'Inner Layer {layer} Copper') for layer in range(1, layer_count-1)],
( pcbnew.B_Cu, 'gbl', 'Back Copper' ),
( pcbnew.B_Mask, 'gbs', 'Back Mask' ),
( pcbnew.B_SilkS, 'gbo', 'Back SilkScreen' ),
( pcbnew.B_Paste, 'gbp', 'Back Paste' ),
( pcbnew.Edge_Cuts, 'gm1', 'Edges Cuts' ),
]
for layer_info in plot_plan:
plot_controller.SetLayer(layer_info[0])
plot_controller.OpenPlotfile('', pcbnew.PLOT_FORMAT_GERBER, layer_info[2])
plot_controller.PlotLayer()
os.rename(dir_fab / f"{project_name}.gbr", dir_fab / f"{project_name}{suffix}.{layer_info[1]}")
plot_controller.ClosePlot()
# ================
# Drill Files
# ================
METRIC = True
ZERO_FORMAT = pcbnew.GENDRILL_WRITER_BASE.DECIMAL_FORMAT
INTEGER_DIGITS = 3
MANTISSA_DIGITS = 3
MIRROR_Y_AXIS = False
HEADER = True
OFFSET = pcbnew.wxPoint(0,0)
MERGE_PTH_NPTH = True
DRILL_FILE = True
MAP_FILE = False
REPORTER = None
drill_writer = pcbnew.EXCELLON_WRITER(pcb)
drill_writer.SetFormat(METRIC, ZERO_FORMAT, INTEGER_DIGITS, MANTISSA_DIGITS)
drill_writer.SetOptions(MIRROR_Y_AXIS, HEADER, OFFSET, MERGE_PTH_NPTH)
drill_writer.CreateDrillandMapFilesSet(str(dir_fab), DRILL_FILE, MAP_FILE, REPORTER)
os.rename(dir_fab / f"{project_name}.drl", dir_fab / f"{project_name}{suffix}.drl")
# ================
# Pick and Place
# ================
# TODO
# ================
# Fab Drawing
# ================
with open(dir_fab / f"README_FABRICATION{suffix}.TXT", "w") as f:
f.write(f"{project_name}-REV{rev}\n")
f.write(f"Layer Order\n")
# for layer in plot_plan:
# ================
# Assembly Drawing
# ================
with open(dir_asy / f"README_ASSEMBLY{suffix}.TXT", "w") as f:
f.write(f"{project_name}-REV{rev}\n")
f.write(f"Layer Order\n")
# for layer in plot_plan: