scripts: Add scripts to generate production files

- The following files can be generated from the script.
1. Zipped(Gerber, Drill, Drill Map)
2. Bom,
3. Component Placement
4. Schematics PDF
5. Step Files

.gitignore

@@ -17,6 +17,8 @@ _autosave-*
 *-save.kicad_pcb
 fp-info-cache
 *auto_saved_files*
+~*
+__pycache__
 
 # Netlist files (exported from Eeschema)
 *.net
@@ -24,3 +26,6 @@ fp-info-cache
 # Autorouter files (exported from Pcbnew)
 *.dsn
 *.ses
+
+# Generated Production Files
+production

scripts/generate_bom_from_xml.py

@@ -0,0 +1,62 @@
+# Modified from "bom_csv_grouped_by_value_with_fp.py" Example BOM Generation Script
+
+"""
+    @package
+    Output: CSV (comma-separated)
+    The BOM does not include components with DNP or excluded from BOM field(s) checked. 
+    Grouped By: Value, Footprint, MFR_PN, MFR_ALT
+    Sorted By: Ref
+    Fields: Ref, Value, MFR_PN, MFR_PN_ALT, Qnty, LibPart, Footprint
+
+    Command line:
+    python "pathToFile/generate_bom_from_xml.py" "%I" "%O.csv"
+"""
+
+import kicad_netlist_reader
+import csv
+import sys
+import os
+
+try:
+    if not os.path.isdir(os.path.dirname(sys.argv[2])):
+        os.makedirs(os.path.dirname(sys.argv[2]))
+    f = open(sys.argv[2], 'w', encoding='utf-8')
+except IOError:
+    raise IOError("Can't open output file for writing: " + sys.argv[2])
+
+# Custom Equal Operator for "groupComponents" method
+def __eq__(self, other):
+    result = False
+    if self.getValue() == other.getValue():
+        if self.getFootprint() == other.getFootprint():
+            if self.getField("MFR_PN") == other.getField("MFR_PN"):
+                if self.getField("MFR_PN_ALT") == other.getField("MFR_PN_ALT"):
+                    result = True
+    return result
+kicad_netlist_reader.comp.__eq__ = __eq__
+
+net = kicad_netlist_reader.netlist(sys.argv[1])
+
+out = csv.writer(f, lineterminator='\n', delimiter=',', quotechar='\"', quoting=csv.QUOTE_ALL)
+out.writerow(['Source:', net.getSource()])
+out.writerow(['Date:', net.getDate()])
+out.writerow(['Tool:', net.getTool()])
+out.writerow(['Ref', 'Value', 'MFR_PN', 'MFR_PN_ALT', 'Qnty', 'LibPart', 'Footprint'])
+
+grouped = net.groupComponents(components=net.getInterestingComponents(excludeBOM=True, DNP=True))
+
+for group in grouped:
+    refs = ""
+    for component in group:
+        if refs != "":
+            refs += ", "
+        refs += component.getRef()
+        c = component
+
+    out.writerow([refs,
+        c.getValue(),
+        c.getField("MFR_PN"),
+        c.getField("MFR_PN_ALT"),
+        len(group),
+        c.getLibName() + ":" + c.getPartName(),
+        c.getFootprint()])

scripts/generate_production_files.py

@@ -0,0 +1,109 @@
+import os
+import argparse
+
+__cmd_get_kicad_bin_path = "which kicad | xargs readlink | sed 's/$/-cli/' | xargs readlink"
+
+def setup_env(prefix, sch, out_dir, dir_kicad_plugins, dir_3d_models):
+    # Get the path to "kicad_netlist_reader.py" script in NixOs
+    if dir_kicad_plugins is None:
+        dir_kicad_plugins = os.path.join(os.popen(__cmd_get_kicad_bin_path).read().replace("\n", ""),
+            "../../share/kicad/plugins")
+    
+    # Setup the PYTHONPATH for "generate_bom_from_xml.py" to import "kicad_netlist_reader"
+    try:
+        pythonpath = os.environ['PYTHONPATH']
+    except KeyError:
+        pythonpath = ''
+    pathlist = [dir_kicad_plugins]
+    if pythonpath:
+        pathlist.extend(pythonpath.split(os.pathsep))
+    os.environ['PYTHONPATH'] = os.pathsep.join(pathlist)
+
+    # NIXOS installs KiCAD Built-in 3D models in a separated folder
+    if dir_3d_models is None:
+        model_3d_path = os.path.join("/nix/store", os.popen("ls /nix/store | grep kicad-packages3d | head -1").read().replace("\n", ""), "share/kicad/3dmodels")
+    # Setup the KICAD7_3DMODEL_DIR for step file to be generated with kicad-cli"
+    os.environ['KICAD7_3DMODEL_DIR'] = model_3d_path
+
+    # Generate the prefix from the title and revision fields in title block of the schematics top
+    if prefix is None:
+        with open (sch, "r") as f:
+            data = f.read().splitlines()
+            title_line = data[7][1:-1].split()
+            revision_line = data[9][1:-1].split()
+        if title_line[0].find("title") and revision_line[0].find("rev"):
+            ret_prefix = f"{title_line[1][1:-1]}_{revision_line[1][1:-1]}"
+        else:
+            raise ValueError("Prefix cannot be generated from schematic file.")
+    else:
+        ret_prefix = prefix
+
+    gerber_drill_dir = os.path.join(out_dir, f"{ret_prefix}_gerber_drill")
+    if not os.path.exists(out_dir):
+        os.makedirs(out_dir)
+    if not os.path.exists(gerber_drill_dir):
+        os.makedirs(gerber_drill_dir)
+
+    return ret_prefix
+
+def generate_production_files(prefix, sch, pcb, out_dir):
+    out_path = os.path.join(out_dir, prefix)
+
+    bom_ret_code = os.system(f"kicad-cli sch export python-bom {sch} -o {out_path}_bom.xml")
+    bom_ret_code |= os.system(f"python -m scripts.generate_bom_from_xml {out_path}_bom.xml  {out_path}_bom.csv")
+    os.system(f"rm {out_path}_bom.xml")
+
+    pdf_ret_code = os.system(f"kicad-cli sch export pdf {sch} -o {out_path}.pdf")
+
+    pos_ret_code = os.system(f"kicad-cli pcb export pos {pcb} --format csv --units mm  -o {out_path}_pos.csv")
+
+    step_ret_code = os.system(f"kicad-cli pcb export step {pcb} --subst-models --force -o {out_path}.step")
+
+    out_path = os.path.join(out_dir, f"{prefix}_gerber_drill")
+    
+    gerber_ret_code = os.system(f"kicad-cli pcb export gerbers {pcb} -l 'F.Cu,In1.Cu,In2.Cu,B.Cu,F.Paste,B.Paste,F.Silkscreen,B.Silkscreen,F.Mask,B.Mask,Edge.Cuts' --no-x2 --subtract-soldermask -o {out_path}")
+    
+    # The additional trailing slash is due to a bug in the kicad-cli tool. https://gitlab.com/kicad/code/kicad/-/issues/14438
+    drill_ret_code = os.system(f"kicad-cli pcb export drill {pcb} -u mm --generate-map --map-format gerberx2 -o {out_path}/")
+    zip_ret_code = os.system(f"zip -r -j {out_path} {out_path}")
+    os.system(f"rm -r {out_path}")
+
+    print("=== File Generation Status === ")
+    print("Gerber: {}".format("Success" if gerber_ret_code == 0 else "Failed"))
+    print("Drill: {}".format("Success" if drill_ret_code == 0 else "Failed"))
+    print("Zip_Gerber_Drill: {}".format("Success" if zip_ret_code == 0 else "Failed"))
+    print("Bom: {}".format("Success" if bom_ret_code == 0 else "Failed"))
+    print("Pdf: {}".format("Success" if pdf_ret_code == 0 else "Failed"))
+    print("Pos: {}".format("Success" if pos_ret_code == 0 else "Failed"))
+    print("Step: {}".format("Success" if step_ret_code == 0 else "Failed"))
+
+def main():
+    parser = argparse.ArgumentParser(
+        description="Python Script to Generate Production Files(Gerber, Drill, Drill Map, Bom, Component Placement, Schematics PDF, Step Files)")
+    parser.add_argument("-s", "--sch",  
+                        default="kirdy.kicad_sch",
+                        help="schematics top file. defaults to 'kirdy.kicad_sch' if omitted")
+    parser.add_argument("-p", "--pcb",  
+                        default="kirdy.kicad_pcb",
+                        help="pcb file. defaults to 'kirdy.kicad_pcb' if omitted")
+    parser.add_argument("-o", "--output",  
+                        default="./production",
+                        help="output folder, defaults to './production' if omitted")
+    parser.add_argument("-pre", "--prefix",  
+                    default=None,
+                    help="output filename prefix, attempts to generated from schematics top file if omitted")
+    parser.add_argument("-dir_plugins", "--dir_kicad_plugins",  
+                default=None,
+                help="path to kicad_netlist_reader.py, attempts to find the required path in the system if omitted")
+    parser.add_argument("-dir_3d", "--dir_3d_models",  
+                default=None,
+                help="path to kicad 3d models folder, attempts to find the required path in the system if omitted")
+
+    args = parser.parse_args()
+
+    prefix = setup_env(args.prefix, args.sch, args.output, args.dir_kicad_plugins, args.dir_3d_models)
+
+    generate_production_files(prefix, args.sch, args.pcb, args.output)
+
+if __name__ == '__main__':
+    main()