Specifications

II Parameters
Base Specifications Parameters
II - 55
【#1072】 chop_ax Chopping axis
Select the chopping axis.
0: Non-chopping axis
1: Chopping axis
【#1073】 I_Absm Initial absolute setting
Select the mode (absolute or incremental) at turning ON the power or reset.
0: Incremental setting
1: Absolute setting
【#1074】 l_Sync Initial synchronous feed
Select the feedrate mode at turning ON the power or reset.
0: Asynchronous feed (feed per minute)
1: Synchronous feed (feed per revolution)
【#1075】 I_G00 Initial G00
Select the linear command mode at turning ON the power or reset.
0: Linear interpolation (G01 command state)
1: Positioning (G00 command state)
【#1076】 Abslnc ABS/INC address (for L system only)
Select the command method for the absolute and incremental commands.
0: Use G command for the absolute and incremental commands.
1: Use axis name for the absolute and incremental commands.
(The axis name in "#1013 axname" will be the absolute command, "#1014 incax" will be
the incremental command.)
When "1" is selected, using two axis names, one each for the absolute and incremental
commands, allows to issue the absolute and incremental commands appropriately to an
axis.
【#1077】 radius Incremental command for diameter specification axis
Select whether the incremental command of the diameter specification axis (“#1019 dia” is
set to “1”) uses the diameter value or radius value.
0: Diameter value
1: Radius value
【#1078】 Decpt2 Decimal point type 2
Select the increment of position commands that do not have a decimal point.
0: Minimum input command unit (follows "#1015 cunit")
1: 1mm (or 1inch) unit (For the dwell time, 1s unit is used.)
【#1079】 F1digt Validate F1 digit
Select the F command method.
0: Direct numerical command (command feedrate during feed per minute or rotation)
1: 1-digit code command (feedrate set with “#1185 spd_F1” to “#1189 spd_F5”)
【#1080】 Dril_Z Specify boring axis (for M system only)
Select a fixed cycle hole drilling axis.
0: Use an axis vertical to the selected plane as hole drilling axis.
1: Use the Z axis as the hole drilling axis regardless of the selected plane.
【#1081】 Gmac_P Give priority to G code parameter
Select the G code priority relationship during the macro call with G command.
0: Priority is on G code used in the system
1: Priority is on registered G code for call
【#1082】 Geomet Geometric
Select the type of geometric to use.
0: Not use
1: Use only geometric I
2: Use geometric I and IB
With geometric, specific address codes are used for exclusive meanings. Thus, if A or C is
used for the axis name or 2nd miscellaneous command code, the A used for the axis name
may function as the geometric's angle designation. Pay special attention to axis names,
etc., when using this function.
【#1084】 RadErr Arc error
Set the tolerable error range when the end point deviates from the center coordinate in the
circular command.
---Setting range---
0 to 1.000 (mm)
【#1085】 G00Drn G00 dry run
Select whether to apply dry run (feed at manual setting speed instead of command
feedrate) to the G00 command.
0: Not apply to G00. (move at rapid traverse rate)
1: Apply to G00. (move at manual setting speed)