202
G CODES
96-8000
June 1999
LIMIT B LOCK B UFFERING F UNCTION (G103)
G103 Limit Block Bufering Group 00
P = 0-15 Max. number of blocks the control will look ahead
G103 [P..]
îš“Block Lookaheadîš” is a term used to describe what the control is doing in the background during machine
motion. A motion block may take several seconds to execute. The control can take advantage of this by
preparing additional blocks of the program ahead of time. Time is saved while the current block is executing
and the next block has already been interpreted and prepared by the continuous, uninterrupted motion be-
tween consecutive blocks. Block lookahead is also important for obtaining information necessary for predicting
compensated positions for cutter compensation.
When G103 P0 is programmed, block limiting is disabled. Block limiting is also disabled if G103 appears in a
block without a P address code.
When G103 Pn is programmed, lookahead is limited to n blocks.
At this time G103 cannot be used if cutter compensation, G41 or G42, is in effect. Alarm 387 is generated if
you attempt to do so.
G103 is also useful for debugging programs using macros. Macro expressions are executed at lookahead
time. By inserting a G103 P1 into the program, macro expressions will be performed one block ahead of the
current executing block.
G103 is not a FANUC compatible command.
CYLINDRICAL M APPING (G107)
G107 Cylindrical Mapping Group 00
X Optional X-axis command A Optional A-axis command
Y Optional Y-axis command Q Optional diameter of cylindrical surface
Z Optional Z-axis command R Optional radius of rotary axis
This G-code translates all programmed motion occurring in a specified linear axis into the equivalent motion
along the surface of a cylinder (attached to a rotary axis). It is a Group 0 G-Code, but its default operation is
subject to Setting 56 (M30 RESTORE DEFAULT G). G107 is used to either activate or deactivate cylindrical
mapping.
* Any linear axis can be cylindrically mapped to any rotary axis (Only one at a time).
* Existing linear-axis G-Code programs can be cylindrically mapped without modification; all that is required is
the prior execution of a single G107 command, which is either placed at the beginning of the G-Code program
itself or, if Setting 56 is set to OFF, can even be specified in a previous G-Code program, provided a RESET
has not been issued in the interim.
To Next Page
Loading...
Need help?
General
