1
0
mirror of git://projects.qi-hardware.com/ben-wpan.git synced 2024-11-25 22:20:37 +02:00
ben-wpan/makefiles/Makefile.kicad
Werner Almesberger 0ee8b42bf1 makefiles/Makefile.kicad: also show drill holes in PNG illustrations
- Makefile.kicad (DRL2GERBER, %-Drill.gbr): convert Excellon drill file to
  Gerber
- Makefile.kicad ($(NAME)-front.png, $(NAME)-back.png,
  $(NAME)-overview.png): use the converted drill file to show holes
- Makefile.kicad (clean): remove $(NAME)-Drill.gbr
2011-03-24 20:06:01 -03:00

201 lines
5.3 KiB
Makefile

#
# Makefile.kicad - Makefile template for KiCAD projects
#
# Written 2011 by Werner Almesberger
# Copyright 2011 Werner Almesberger
#
# This program is free software; you can redistribute it and/or modify
# it under the terms of the GNU General Public License as published by
# the Free Software Foundation; either version 2 of the License, or
# (at your option) any later version.
#
#
# Define before including this template:
#
# NAME project name
# VERSION "release" version number
#
PLOT_BRD = pcbnew --plot=ps_a4 --ps-pads-drill-opt=none --fill-all-zones
CPTX = ../../eda-tools/mlztx/cptx
GMERGE = ../../eda-tools/fab/gmerge
DRL2GERBER = ../../eda-tools/fab/drl2gerber
PRETTYGERBV = ../../eda-tools/fab/prettygerbv
POS2FAB = ../../eda-tools/fab/pos2fab
FPDOC = PATH=$$PATH:../../eda-tools/fab:../../eda-tools/fpd2pdf fpdoc
DIR = $(shell pwd | sed 's|.*/||')
SCH=$(shell pwd)/$(NAME).sch
BRD=$(shell pwd)/$(NAME).brd
.PHONY: all gen generate sch brd xpdf front back clean
.PHONY: gerber gerbv fab fab-pcb fab-smt overview
all:
@echo "make what ? target: gen sch brd xpdf front back clean"
@exit 1
gen generate:
eeschema --plot=ps $(SCH)
# need scripts
sch:
eeschema $(SCH)
brd:
pcbnew $(BRD)
xpdf:
xpdf $(NAME).pdf
front: $(NAME)-Front.ps
lpr $<
back: $(NAME)-Back.ps
lpr $<
# --- DIY production (toner transfer) -----------------------------------------
#
# Postscript for production of front/back layer, using the toner transfer
# method. Note that other artwork transfer methods may require different
# mirror settings.
#
# We use --ps-pads-drill-opt=none to avoid having any hole before drilling,
# which yields the best results with a CNC drill. For manual drilling, "real"
# would be preferrable. Do not use "small", for this created holes that are
# larger (!) than designed.
#
%-Front.ps: %.brd
$(PLOT_BRD) -l Front --mirror $<
%-Back.ps: %.brd
$(PLOT_BRD) -l Back $<
# --- Industrial production ---------------------------------------------------
GERBERS = $(NAME)-SilkS_Front.gto $(NAME)-Mask_Front.gts \
$(NAME)-Front.gtl $(NAME)-Back.gbl $(NAME)-Mask_Back.gbs \
$(NAME)-PCB_Edges.gbr $(NAME)-SoldP_Front.gtp
PCB_FILES = README-PCB $(NAME)-front.png $(NAME)-back.png \
$(NAME)-PCB_Edges.dxf $(NAME).drl $(GERBERS)
SMT_FILES = README-SMT $(NAME)-front.png $(NAME)-bom.csv $(NAME)-pos.csv \
$(NAME)-footprints.pdf
gerber: $(GERBERS)
$(GERBERS): $(NAME).brd Makefile
pcbnew --plot=gerber --origin=aux \
-l `pcbnew --list-layers $(BRD) | tr '\012' ,` \
--fill-all-zones --exclude-pcb-edge \
$(BRD)
$(GMERGE) $(NAME)-SilkS_Front.gto $(NAME)-Comments.gbr >_tmp \
|| { rm -rf _tmp; exit 1; }
mv _tmp $(NAME)-SilkS_Front.gto
fab: fab-pcb fab-smt
$(NAME)-PCB_Edges.dxf: $(NAME).brd
pcbnew --plot=dxf --origin=aux -l PCB_Edges $(BRD)
$(NAME).drl: $(NAME).brd
pcbnew --drill --origin=aux $(BRD)
fab-pcb: $(PCB_FILES)
mkdir -p fab
tar Ccfz .. fab/$(NAME)-pcb-$(VERSION).tar.gz \
$(PCB_FILES:%=$(DIR)/%)
cd ..; zip -l $(DIR)/fab/$(NAME)-pcb-$(VERSION).zip \
$(PCB_FILES:%=$(DIR)/%)
gerbv:
gerbv $(NAME)-SilkS_Front.gto \
$(NAME)-SoldP_Front.gtp \
$(NAME)-Front.gtl \
$(NAME)-Mask_Front.gts \
$(NAME)-Mask_Back.gbs \
$(NAME)-Back.gbl \
$(NAME)-PCB_Edges.gbr
$(NAME)Front.pos:
pcbnew --pos $(BRD)
%-pos.csv: %Front.pos %.cmp
$(POS2FAB) $^ >$@ || { rm -f "$@"; exit 1; }
../bom/$(NAME)-bom.csv:
$(MAKE) -C ../bom $(NAME)-bom.csv
%-bom.csv: ../bom/%-bom.csv
mv $< $@
%-footprints.pdf: %.pro %.cmp %Front.pos
$(FPDOC) -a FIDUCIAL $< "$@" || { rm -f "$@"; exit 1; }
fab-smt: $(SMT_FILES)
mkdir -p fab
tar Ccfz .. fab/$(NAME)-smt-$(VERSION).tar.gz \
$(SMT_FILES:%=$(DIR)/%)
cd ..; zip -l $(DIR)/fab/$(NAME)-smt-$(VERSION).zip \
$(SMT_FILES:%=$(DIR)/%)
upload:
qippl \
fab/$(NAME)-pcb-$(VERSION).tar.gz \
fab/$(NAME)-pcb-$(VERSION).zip \
fab/$(NAME)-smt-$(VERSION).tar.gz \
fab/$(NAME)-smt-$(VERSION).zip \
wpan/fab
# --- Overview images ---------------------------------------------------------
%-Drill.gbr: %.drl
$(DRL2GERBER) $^ >$@ || { rm -f "$@"; exit 1; }
$(NAME)-front.png: gerber $(NAME)-Drill.gbr
$(PRETTYGERBV) -d $(NAME)-Drill.gbr $(NAME) front \
$(NAME)-front.png
$(NAME)-back.png: gerber $(NAME)-Drill.gbr
$(PRETTYGERBV) -d $(NAME)-Drill.gbr $(NAME) back \
$(NAME)-back.png
$(NAME)-overview.png: gerber $(NAME)-Drill.gbr
$(PRETTYGERBV) -d $(NAME)-Drill.gbr $(NAME) all \
$(NAME)-overview.png
overview: $(NAME)-overview.png
display $(NAME)-overview.png
uoverview: $(NAME)-overview.png
qippl $(NAME)-overview.png \
wpan/tmp/$(NAME)-$(VERSION)-overview.png
# --- Cleanup -----------------------------------------------------------------
clean::
rm -f $(NAME)-Front.ps $(NAME)-Back.ps
rm -f $(NAME).drl $(NAME)-Drill.gbr
rm -f $(NAME)-PCB_Edges.gbr $(NAME)-PCB_Edges.dxf
rm -f $(NAME)-Front.gtl $(NAME)-Mask_Front.gts
rm -f $(NAME)-SilkS_Front.gto $(NAME)-SoldP_Front.gtp
rm -f $(NAME)-Back.gbl $(NAME)-Mask_Back.gbs
rm -f $(NAME)-SilkS_Back.gbo $(NAME)-SoldP_Back.gbp
rm -f $(NAME)-Comments.gbr $(NAME)-Drawings.gbr
rm -f $(NAME)-overview.png $(NAME)-front.png $(NAME)-back.png
rm -f $(NAME)Front.pos $(NAME)-pos.csv
rm -f $(NAME)-bom.csv $(NAME)-footprints.pdf
spotless:: clean
rm -f '$$'savepcb.000 '$$'savepcb.brd
rm -f $(NAME)-cache.lib $(NAME)-cache.bak
rm -f $(NAME).000
rm -f $(NAME).net