# *****************************************************************************
# *   Copyright (c) 2020 Rene 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                                                                     *
# *                                                                           *
# ****************************************************************************/
"""Postprocessor to output real GCode for Max Computer GmbH nccad9."""
import FreeCAD
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 output 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 !!!

import nccad_post
nccad_post.export([object], "/path/to/file.knc", "")
"""

MACHINE_NAME = """Max Computer GmbH nccad9 MCS/KOSY"""

# gCode for changing tools
# M01 <String> ; Displays <String> and waits for user interaction
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 spindle"""


# 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
if FreeCAD.ActiveDocument:
    cam_file = FreeCAD.ActiveDocument.FileName
else:
    cam_file = "<None>"

HEADER = """;Exported by FreeCAD
;Post Processor: {}
;CAM file: {}
;Output Time: {}
""".format(
    __name__, cam_file, str(datetime.datetime.now())
)


def export(objectslist, filename, argstring):
    """Export the list of objects into a filename.

    Parameters
    ----------
    objectslists: list
        List of objects.

    filename: str
        Name of the output file ending in `'.knc'`.
    """
    gcode = HEADER

    for obj in objectslist:
        for command in obj.Path.Commands:
            # Manipulate tool change commands
            if "M6" == command.Name:
                gcode += TOOL_CHANGE.replace("TOOL", str(int(command.Parameters["T"])))
            elif "M3" == command.Name:
                # Convert spindle speed (rpm) command to comment
                gcode += (
                    "M01 Set spindle speed to "
                    + str(int(command.Parameters["S"]))
                    + " rounds per minute"
                )
            else:
                # Add other commands
                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 and round float
                    # as nccad9 does not support exponents
                    gcode += " " + parameter + str(round(value, 5))

            gcode += "\n"

    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 filename != "-":
        gfile = open(filename, "w")
        gfile.write(gcode)
        gfile.close()

    return filename
