mirror of
https://github.com/oresat/oresat-adcs-hardware.git
synced 2026-03-19 11:06:04 +00:00
cbe040fa59
Updated schematic symbols, cleaned up schematic pages to be more like protocard, removed uncessessary TPs, updated layout, cleaned up layout routing and some zones, added Makefile and READMEs for fabrication. Only BOM formatting left!
99 lines
5.1 KiB
Makefile
99 lines
5.1 KiB
Makefile
# Build automation for KiCad projects
|
|
#
|
|
# Type "make" to output all of the fabrication and assembly files you'll need into a directory called 'build'.
|
|
#
|
|
# The makefile automatically looks for a local *.kicad_pro file and assumes that's your project name. It
|
|
# then assumes you want your build products to go into a folder called "build", of course.
|
|
#
|
|
# Note: PRESET_NAME is the preset for your BOM format. kicad-cli will happily output a completely useless BOM
|
|
# of just REF, VALUE, FOOTPRINT, that's it, unless you set up the BOM tool with a "preset". We suggest you create
|
|
# 'bom-preset' when working in KiCad which has "all the things" when you're editing the schematic, and then
|
|
# another preset called 'bom-export-preset' when exporting your BOM into a CSV file. This export preset removes
|
|
# VALUE, FOOTPRINT, and DATASHEET.
|
|
|
|
PROJECT_FILE = $(firstword $(shell echo *.kicad_pro))
|
|
PROJECT_NAME = $(PROJECT_FILE:%.kicad_pro=%)
|
|
SCHEMATIC = $(PROJECT_NAME).kicad_sch
|
|
BOARD = $(PROJECT_NAME).kicad_pcb
|
|
TIMESTAMP = $(shell date '+%Y-%m-%dT%H-%M-%S')
|
|
PRESET_NAME ?= bom-export-preset
|
|
OUTPUT_DIR ?= build
|
|
DOC_DIR ?= documentation
|
|
FAB_DIR ?= fabrication
|
|
ASM_DIR ?= assembly
|
|
CAD_DIR ?= cad
|
|
|
|
# Default target (first target is default)
|
|
all: erc pdf bom drc ipc gbr drl pos jpg dxf stp rme cad zip
|
|
|
|
# Build all but skip ERC and DRC checks. It's called fafo for a reason, kids.
|
|
fafo: pdf bom ipc gbr drl pos jpg dxf stp rme cad zip
|
|
|
|
# Generate build files from the schematic
|
|
|
|
erc: ## Check for errors and warnings. Exit build if you have any. Remove the useless report if none.
|
|
kicad-cli sch erc -o $(OUTPUT_DIR)/$(DOC_DIR)/$(PROJECT_NAME)-erc.rpt --severity-error --severity-warning --exit-code-violations $(SCHEMATIC)
|
|
rm -f $(OUTPUT_DIR)/$(DOC_DIR)/$(PROJECT_NAME)-erc.rpt
|
|
|
|
pdf: ## Generate a PDF of the schematic
|
|
kicad-cli sch export pdf -o $(OUTPUT_DIR)/$(DOC_DIR)/$(PROJECT_NAME)-schematic.pdf $(SCHEMATIC)
|
|
|
|
bom: ## Generate a CSV Bill of Materials (BOM) with the output preset file that you created in your schematic.
|
|
kicad-cli sch export bom --preset $(PRESET_NAME) -o $(OUTPUT_DIR)/$(ASM_DIR)/$(PROJECT_NAME)-bom.csv $(SCHEMATIC)
|
|
|
|
# Generate build files from the board
|
|
|
|
drc: ## Check layout for schematic parity, layout errors, and layout warnings. Exit build if there are any. Remove useless report if none.
|
|
kicad-cli pcb drc -o $(OUTPUT_DIR)/$(FAB_DIR)/$(PROJECT_NAME)-drc.rpt --schematic-parity --severity-error --severity-warning --exit-code-violations $(BOARD)
|
|
rm -f $(OUTPUT_DIR)/$(FAB_DIR)/$(PROJECT_NAME)-drc.rpt
|
|
|
|
ipc: ## IPC-2581 is an open standard used for board fab and assembly (silly to copy it twice, but :shrug:
|
|
kicad-cli pcb export ipc2581 -o $(OUTPUT_DIR)/$(FAB_DIR)/$(PROJECT_NAME)-ipc2581.xml $(BOARD)
|
|
cp $(OUTPUT_DIR)/$(FAB_DIR)/$(PROJECT_NAME)-ipc2581.xml $(OUTPUT_DIR)/$(ASM_DIR)/
|
|
|
|
gbr: ## Modern Gerber files for all the standard layers (kill the jobs file)
|
|
kicad-cli pcb export gerbers -o $(OUTPUT_DIR)/$(FAB_DIR) --board-plot-params $(BOARD)
|
|
rm -f $(OUTPUT_DIR)/$(FAB_DIR)/*.gbrjob
|
|
cp $(OUTPUT_DIR)/$(FAB_DIR)/*_Paste.gbr $(OUTPUT_DIR)/$(ASM_DIR)/
|
|
|
|
drl: ## Excellon drill files, separated by plated / non-plated holes which is sometimes useful
|
|
kicad-cli pcb export drill -o $(OUTPUT_DIR)/$(FAB_DIR) --excellon-separate-th $(BOARD)
|
|
|
|
pos: ## Position files for pick and place machines (also in the ipc file)
|
|
kicad-cli pcb export pos -o $(OUTPUT_DIR)/$(ASM_DIR)/$(PROJECT_NAME).pos --exclude-dnp $(BOARD)
|
|
|
|
# Generate renders of the board
|
|
|
|
jpg: ## Generate photorealistic renders of the top and bottom sides of the PCB
|
|
kicad-cli pcb render -o $(OUTPUT_DIR)/$(DOC_DIR)/$(PROJECT_NAME)-render-top.jpg --side top -w 3840 -h 2160 $(BOARD)
|
|
kicad-cli pcb render -o $(OUTPUT_DIR)/$(DOC_DIR)/$(PROJECT_NAME)-render-bot.jpg --side bottom -w 3840 -h 2160 $(BOARD)
|
|
|
|
dxf: ## DXF drawing of the board outline, with cutouts and larger holes
|
|
kicad-cli pcb export dxf -o $(OUTPUT_DIR)/$(DOC_DIR)/$(PROJECT_NAME)-outline.dxf --mode-single -l Edge.Cuts $(BOARD)
|
|
|
|
stp: ## A 3D STEP file to import into your MCAD package
|
|
kicad-cli pcb export step -o $(OUTPUT_DIR)/$(DOC_DIR)/$(PROJECT_NAME)-pcba.step --no-dnp --include-silkscreen --include-soldermask --include-pads --cut-vias-in-body $(BOARD)
|
|
|
|
rme: ## Readme files
|
|
cp README-fabrication.md $(OUTPUT_DIR)/$(FAB_DIR)
|
|
cp README-assembly.md $(OUTPUT_DIR)/$(ASM_DIR)
|
|
|
|
cad: ## CAD files
|
|
mkdir -p $(OUTPUT_DIR)/$(CAD_DIR)
|
|
cp *.kicad_pro *.kicad_sch *.kicad_pcb $(OUTPUT_DIR)/$(CAD_DIR)
|
|
|
|
zip: ## Zip the file with a timestamp (one for everything, and one for each directory)
|
|
|
|
zip -r $(OUTPUT_DIR)/$(PROJECT_NAME)-$(TIMESTAMP).zip $(OUTPUT_DIR)/*
|
|
zip -r $(OUTPUT_DIR)/$(PROJECT_NAME)-$(TIMESTAMP)-$(DOC_DIR).zip $(OUTPUT_DIR)/$(DOC_DIR)/*
|
|
zip -r $(OUTPUT_DIR)/$(PROJECT_NAME)-$(TIMESTAMP)-$(FAB_DIR).zip $(OUTPUT_DIR)/$(FAB_DIR)/*
|
|
zip -r $(OUTPUT_DIR)/$(PROJECT_NAME)-$(TIMESTAMP)-$(ASM_DIR).zip $(OUTPUT_DIR)/$(ASM_DIR)/*
|
|
zip -r $(OUTPUT_DIR)/$(PROJECT_NAME)-$(TIMESTAMP)-$(CAD_DIR).zip $(OUTPUT_DIR)/$(CAD_DIR)/*
|
|
|
|
clean: ## delete everything for clean
|
|
rm -rf $(OUTPUT_DIR)/*
|
|
|
|
# Tell make that these are commands, not files
|
|
.PHONY: all fafo erc pdf bom drc ipc gbr drl pos jpg dxf stp rme cad zip clean
|
|
|