Add basic Max Computer GmbH nccad9 postprocessor

This is a postprocessor file for the Path workbench. It is used to take a pseudo-gcode fragment outputted by a Path object and output real GCode suitable for the Max Computer GmbH nccad9 Computer Numeric Control used in german (vocational) schools.

Supported features:
- 3-axis milling
- manual tool change with tool number as comment
- spindle speed as comment

gCode files must use the suffix .knc !!!

src/Mod/Path/PathScripts/post/nccad_post.py

@@ -0,0 +1,122 @@
+# *********************************************************************************************
+# *   Copyright (c) 2019/2020 Rene 'Renne' Bartsch, B.Sc. Informatics <rene@bartschnet.de>    *
+# *                                                                                           *
+# *   This file is part of the FreeCAD CAx development system.                                *
+# *                                                                                           *
+# *   This program is free software; you can redistribute it and/or modify                    *
+# *   it under the terms of the GNU Lesser General Public License (LGPL)                      *
+# *   as published by the Free Software Foundation; either version 2 of                       *
+# *   the License, or (at your option) any later version.                                     *
+# *   for detail see the LICENCE text file.                                                   *
+# *                                                                                           *
+# *   FreeCAD is distributed in the hope that it will be useful,                              *
+# *   but WITHOUT ANY WARRANTY; without even the implied warranty of                          *
+# *   MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE.  See the                           *
+# *   GNU Lesser General Public License for more details.                                     *
+# *                                                                                           *
+# *   You should have received a copy of the GNU Library General Public                       *
+# *   License along with FreeCAD; if not, write to the Free Software                          *
+# *   Foundation, Inc., 59 Temple Place, Suite 330, Boston, MA  02111-1307                    *
+# *   USA                                                                                     *
+# *                                                                                           *
+# ********************************************************************************************/
+import FreeCAD
+import PathScripts
+from PathScripts import PostUtils
+import datetime
+
+
+TOOLTIP='''
+This is a postprocessor file for the Path workbench. It is used to take
+a pseudo-gcode fragment outputted by a Path object and output real GCode
+suitable for the Max Computer GmbH nccad9 Computer Numeric Control.
+
+Supported features:
+
+- 3-axis milling
+- manual tool change with tool number as comment
+- spindle speed as comment
+
+!!! gCode files must use the suffix .knc !!!'''
+
+
+MACHINE_NAME = '''Max Computer GmbH nccad9 MCS/KOSY'''
+
+
+# gCode for changing tools
+TOOL_CHANGE = '''G77      ; Move to release position
+M10 O6.0 ; Stop spindle
+M01 Insert tool TOOL
+G76      ; Move to reference point to ensure correct coordinates after tool change
+M10 O6.1 ; Start spindel'''
+
+
+# gCode finishing the program
+POSTAMBLE = '''G77      ; Move to release position
+M10 O6.0 ; Stop spindle'''
+
+
+# gCode header with information about CAD-software, post-processor and date/time
+HEADER = ''';Exported by FreeCAD
+;Post Processor: {}
+;CAM file: {}
+;Output Time: {}
+'''.format(__name__, FreeCAD.ActiveDocument.FileName, str(datetime.datetime.now()))
+
+
+# Post processing function
+def export(objectslist, filename, argstring):
+
+  # Add header with description
+  gcode = HEADER
+
+  # Loop through path objects
+  for obj in objectslist:
+
+    # Loop through command objects
+    for command in obj.Path.Commands:
+
+      # Manipulate tool change commands
+      if 'M6' == command.Name:
+        gcode += TOOL_CHANGE.replace('TOOL', str(int(command.Parameters['T'])))
+
+      # Convert spindle speed (rpm) command to comment
+      elif 'M3' == command.Name:
+        gcode += 'M01 Set spindle speed to ' + str(int(command.Parameters['S'])) + ' rounds per minute'
+
+      # Add other commands
+      else:
+        gcode += command.Name
+
+        # Loop through command parameters
+        for parameter, value in command.Parameters.items():
+
+          # Multiply F parameter value by 10 (FreeCAD = mm/s, nccad = 1/10 mm/s)
+          if 'F' == parameter:
+            value *= 10
+
+          # Add command parameters and values
+          gcode += ' ' + parameter + str(round(value, 5))
+
+      # Add line-break of command
+      gcode += '\n'
+
+  # Add postamble
+  gcode += POSTAMBLE + '\n'
+
+  # Open editor window
+  if FreeCAD.GuiUp:
+    dia = PostUtils.GCodeEditorDialog()
+    dia.editor.setText(gcode)
+    result = dia.exec_()
+    if result:
+      gcode = dia.editor.toPlainText()
+
+  # Save to file
+  if not filename == '-':
+    gfile = open(filename, "w")
+    gfile.write(gcode)
+    gfile.close()
+
+  # Return
+  return filename