Interpreter

\[interpreter] initialstring 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 dualqueueenabled 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 g4inmilliseconds 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 longfilemodecriterion 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 superlongfilemodecriterion 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 macrofilename macro file name name of the macro file the default is macro cnc diameterprogramming (turning machine only) 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) absolutecentercoords (turning machine only) 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 fullcirclethetaepsilon 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 reverseg2g3 swap g2 and g3 swaps functionality of g2 (clockwise arc) and g3 (counter clockwise arc) commands this is commonly done for turning machines nohaltfortoolchange run change tool subroutine on m6 command / do not pause for tool change if enabled, the machine will run the change tool subroutine from the macro and not wait for tool changes when this setting is disabled, the machine will pause when an m6 command is executed to change the tool manually 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 tanknifeangleforliftup (tangential knife cutter only) 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 tanknifeblendangle (tangential knife cutter only) 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 tanknifeblenddistance (tangential knife cutter only) 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 tanknifeliftupdistance (tangential knife cutter only) tangential knife lift up distance specifies the distance to lift up z when the detected angle is greater than the tangential knife bending angle tanknifebendingangle (tangential knife cutter only) tangential knife bending angle defines the direction to which the knife is angled towards for 45° knives tanknifezhi (tangential knife cutter only) 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 tanknifezlo (tangential knife cutter only) 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 tankniferewindturns (tangential knife cutter only) 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 timeestimatefactor job time estimation factor estimated job time is adjusted by this factor simplezeroing 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 useg10l20forzeroing 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