# 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