Interpreter
G-Code to be executed on start G-Code to be executed on software start. One line only.
This setting can be used to set the default/safe state of the machine, e.g. set a default feed rate with F100.
Only G-Code can be used. Interpreter commands such as tcaguard on cannot be used here. You can put such commands in (as an example) home_all subroutine instead.
Dual queue Determines if dual queue feature is enabled. Dual queue feature utilizes a second motion queue to be able to provide motion while the main queue already contains data. Meaning that, it enables interpreter commands to be executed (e.g. M3) while a job is paused.
When dual queue is enabled, toggles for hardware actions (e.g. Tool/Spindle on/off button, Flood on/off button) will utilize respective M-Codes (e.g. M3, M8) instead of directly switching respective output on/off. This is usually desirable because it means that these UI elements will respect overriden M-Codes. For that reason, it is recommended to leave this setting enabled.
G4 parameter is in milliseconds Indicates that the P-value used with G4 is to be interpreted as milliseconds. By default, this value is in seconds.
Long file mode threshold [kB] Job file size that when exceeded will trigger "Long file mode".
In "Long file mode", the job file will not be shown in its entirety. This is done to preserve system memory and improve performance.
If there are noticeable performance issues, computer input delays or the machine is not functioning properly when large file jobs are run, it is advised to lower this value.
Super long file mode threshold [kB] Job file size that when exceeded will trigger "Super long file mode".
In "Super long file mode", the job file will not be shown in its entirety. The file will also no longer be loaded into system's memory in it's entirety, which means that complex G-Code constructs (while, if-then-else, macro subroutines) are no longer possible. This is done to preserve system memory and improve performance. Theoretically, files of any size can be executed in this mode.
If there are noticeable performance issues, computer input delays or the machine is not functioning properly when large file jobs are run, it is advised to lower this value.
Macro file name Name of the macro file. The default is macro.cnc.
Diameter programming for lathe machines Enables diameter programming mode for turning machines. In diameter programming mode, all X-axis values are interpreted as a diameter (all movements in the X-axis are divided by 2).
G2/G3 center coordinates are absolute Enables interpretation of G2 and G3 center coordinates as absolute values. If this setting is disabled, the values are interpreted as incremental.
Full circle theta epsilon Factor value for treating arcs as full circles.If the distance between start and end point of a circle is less than this value, the circle is considered to be full.
Swap G2 and G3 Swaps functionality of G2 (clockwise arc) and G3 (counter-clockwise arc) commands. This is commonly done for turning machines.
Do not pause for tool change If enabled, the machine will not stop for tool changes.
It is not recommended to use this setting if you do not have an Automatic Tool Changer (ATC). If you have an ATC and it is set up (change_tool subroutine is working properly with your tool changer), enabling this setting will skip the forced tool change stop.
Tangential knife safe angle threshold The angle between two movements that will trigger a Z-axis lift when exceeded, in order to rotate the knife safely. If the angle is lower, the knife is rotated during motion, without lifting it up.
The tangential knife is switched on through interpreter commands and can be configured by interpreter commands as well. Please consult the manual for more information.
Tangential knife blend angle
When angle between subsequent motion segments is less than this value, the knife is not rotated before the angle but during motion. The motion segments also have to be shorter than the tangential knife blend distance.
For small angles in combination with small motion segments, this is tolerable in practice and will speed up the cutting process a lot. Be aware however that the knife direction is not exactly in the cutting direction and the knife may break if the angle is too large. It is advised to only use this with small angles.
Tangential knife blend distance When subsequent motion segments (or arc length) are shorter than this value, the knife is not rotated before an angle but during motion. The angle between the motion segments also has to be less than the tangential knife blend angle.
Tangential knife lift up distance Specifies the distance to lift up Z when the detected angle is greater than the tangential knife bending angle.
Tangential knife bending angle Defines the direction to which the knife is angled towards for 45° knives.
Tangential knife ZHI value Define the high Z position in work coordinates for 45° knives.
Usually, this is 1-5mm above the material. This setting requires careful calibration. Please consult the manual.
Tangential knife ZLO value Define the low Z value in work coordinates for 45° knives.
This is the deepest point in the cut groove. This setting requires careful calibration. Please consult the manual.
Tangential knife turns to rewind Specifies the number of turns after which the knife will be rotated back.
This prevents issues related to the knife rotating too much in one direction, e.g. with wires.
Job time estimation factor Estimated job time is adjusted by this factor.
Simple zeroing Enables simplified work coordinate zeroing. If enabled, the zero buttons in the operate view, will simply set the work position to zero at the current position. Otherwise, a dialog will be shown in which the position can be set.
By default, the dialog shows a value which is reduced by tool radius of the current tool. This is handy when zeroing from the lower-left corner with the end mill against the material.
Use G10L20 for zeroing If enabled, the active coordinate system (G54 – G59.3) is zeroed instead of the global G92. Otherwise, the global G92 offset is used.