# Section and variable names must be valid Python identifiers
# do not use whitespace in names
# do not edit the following section name:
[Version]
# do not edit the following value:
config_version = 6
[General]
# This extension is used in the save file export dialog.
output_format = .ngc
# This title is shown in the export dialog and is used by the user to differentiate between the possible different postprocessor configurations.
output_text = G-CODE for LinuxCNC
# This type defines the output format used in the export dialog.
output_type = g-code
# Used to switch between absolute (G90) and relative/incremental coordinates (G91).
abs_export = True
# If cutter compensation is used, e.g. G41 or G42, this option cancels the compensation when there is a momevement on the 3rd-axis, and enables the compensation again afterwards.
cancel_cc_for_depth = False
# If cutter compensation is used (G41-G42) this will apply the cutter compensation outside the piece (i.e. it is applied before it is at milling depth).
cc_outside_the_piece = True
# Used for dxfs which only support arcs that are in counterclockwise direction. Turning this on for normal G-Code will result in unintended output.
export_ccw_arcs_only = False
# If an arc's radius exceeds this value, then it will be exported as a line.
max_arc_radius = 10000.0
code_begin_units_mm = G21 (Units in millimeters)
code_begin_units_in = G20 (Units in inches)
code_begin_prog_abs = G90 (Absolute programming)
code_begin_prog_inc = G91 (Incremental programming)
# This is code which will be written at the beginning of the exported file.
code_begin = G64 (Default cutting) G18 (XZ plane) G40 (Cancel radius comp.) G49 (Cancel length comp.)
# This is code which will be written at the end of the exported file.
code_end = M2 (Program end)
[Number_Format]
# Gives the indentation for the values.
pre_decimals = 4
# Gives the accuracy of the output after which it will be rounded.
post_decimals = 3
# Give the separator which is used in the exported values (e.g. '.' or ',').
decimal_separator = .
# If true all values will be padded with zeros up to pre_decimals (e.g. 0001.000).
pre_decimal_zero_padding = False
# If false e.g. 1.000 will be given as 1 only.
post_decimal_zero_padding = True
# If True 1.000 will be written as +1.000
signed_values = False
[Line_Numbers]
# Enables line numbers into the exported G-Code file.
use_line_nrs = False
line_nrs_begin = 10
line_nrs_step = 10
[Program]
# This will be done after each layer, if different tools are used.
tool_change = T%tool_nr M6%nlS%speed%nl
# This will be done after each change between cutting in plane or cutting in depth.
feed_change = F%feed%nl
# This will be done between each shape to cut.
rap_pos_plane = G0 X%YE Z%XE%nl
# This will be done between each shape to cut.
rap_pos_depth = G0 Y%ZE %nl
# This will be used for shape cutting.
lin_mov_plane = G1 X%YE Z%XE%nl
# This will be used for shape cutting.
lin_mov_depth = G1 Y%ZE%nl
# This will be used for shape cutting.
arc_int_cw = G2 X%YE Z%XE R%R%nl
# This will be used for shape cutting.
arc_int_ccw = G3 X%YE Z%XE R%R%nl
# Generally set to G40%nl
cutter_comp_off = G40%nl
# Generally set to G41%nl
cutter_comp_left = G41%nl
# Generally set to G42%nl
cutter_comp_right = G42%nl
# This will be done before starting to cut a shape or a contour.
pre_shape_cut = M3 M8%nl
# This will be done after cutting a shape or a contour.
post_shape_cut = M9 M5%nl
# Defines comments' format. Comments are written at some places during the export in order to make the g-code better readable.
comment = %nl(%comment)%nl
