Option File Generator HelpCycles
This option controls whether the Z value in cycle blocks is output in absolute or incremental mode. The Z value can be output several ways:
As an absolute coordinate in a cycle block
As an incremental value measured from the rapid stop point.
As an absolute incremental value measured from the rapid stop point.
Equivalent postprocessor commands:
PLABEL./OPTION,41,TO,0 $$ Output Z as absolute value (default).
PLABEL./OPTION,41,TO,1 $$ Output Z as incremental value.
PLABEL./OPTION,41,TO,2 $$ Output Z as absolute incremental value.
Some controllers automatically add a retract clearance value for the R plane. Entering a value in this box will automatically subtract this value from the value programmed as the clearance plane in the CYCLE commands.
You can selectively control the output of the linear and /or rotary registers that have the same value under cycle G81 type motion. The cycle axis data (R, Z) will always be output for the first point.
Some imported controllers have built-in retract capabilities that cause a crash condition if the postprocessor performs motion analysis and outputs a CYCLE/OFF code. Do not check this box if you wish to suppress the motion analysis and force out cycle motion in one block. Equivalent postprocessor commands:
PLABEL/OPTION,44,TO,0 $$ Default CYCLE motion analysis (default).
PLABEL/OPTION,44,TO,1 $$ CYCLE motion in one block.
Check this box if a positive Z move retracts the tool away from the work piece. Do not check this box if a positive Z move advances the tool toward the work piece.
Enter the letter address of the retracting axis.
Specify the letter address to output the DEEP cycle INCR value given in the part program. Select "Disable" if this increment value is manually set at the machine tool.
Some machine tools have an option to dwell during a fixed cycle. The dwell time is specified in the cycle block using a special letter address. The LOCK option in cycle commands in the part program will generate the required dwell value. Select "Disable"if your control does not recognize this feature.
The address specified for cycle cam will be used to output the stop values for fixed cycles. The CAM option in cycle commands in the part program will generate the required cam number. Select "Disable" if your control does not recognize this feature.
Specify the letter address to output the Secondary Clearance Plane value for all canned cycles. Select "Disable" if your controller does not have a Secondary Clearance Plane. The Secondary clearance plane value c2 is given in the CYCLE command as CYCLE/--,RTRCTO,c2. Using this option, you specify if c2 is incremental or absolute from the cycle goto point. When set to absolute, you can retract to a known z-height regardless of the z-height of the drill point.
--------------------------------------------------------------------------------------------------------------------------
Option File Generator Help
Copyright (c) 2005, All Rights Reserved,
Austin N.C., 505 East Huntland Drive, Suite 480
Austin, TX 78752
www.austinnc.com