Option File Generator HelpGeneral
Check this box if your controller does not have G2/G3 circular interpolation. The circles will be converted into G1 linear moves that iterate the arc. Checking this will disable the Clockwise Prep and CCW Prep fields.
Enter the numeric value that sets clockwise interpolation. Enter NR (not required) if no preparatory code is required. This response suppresses the output of the preparatory code without turning off circular interpolation. If this machine is not capable of circular interpolation at all, enter NA (not available).
Enter the numeric value that sets counterclockwise interpolation. Enter NR (not required) if no preparatory code is required. This response suppresses the output of the preparatory code without turning off circular interpolation. If this machine is not capable of circular interpolation at all, enter NA (not available).
Some controllers require that circular preparatory codes be output on each block. Others retain the current preparatory code as modal. Modal codes are output only when their value changes, not on every block.
Some controllers require axis motion registers to be output on each circular block. Others retain the current value as modal. Modal codes are output only when their values change, not on every block.
Circular interpolation blocks may represent the radius or radius center in one of four ways. The machine may use two registers to locate the radius center relative to the tool tip. In that case, choose I/K to select ARC OFFSET. If the machine uses a single register containing the actual radius for the circular motion, choose RADIUS to select RADIUS programming. Equivalent postprocessor commands:
PLABEL/OPTION,94,TO,0 $$ Output IJK with circular G-codes (default).
PLABEL/OPTION,94,TO,1 $$ Output R with circular G-codes.
Additional options that are slight modifications to the above two options are shown below:
PLABEL/OPTION,94,TO,2 $$ Output +R if angle is < 180 ; Output –R if angle is > 180
PLABEL/OPTION,94,TO,3 $$Output +R if angle is < 180 ; Output –R if angle is > 180 ; Output IJK if angle = 360
If your machine requires a new block to be output at each quadrant crossing, select the the Default quadrant crossing option. Otherwise, if circular records are not required at each quadrant crossing select one of the other options. Equivalent postprocessor commands:
PLABEL/OPTION,93,TO,0 $$ Default circular interpolation. Circle records break at every quadrant crossing (default).
If your machine control does not require the postprocessor to break the motion into individual blocks at each quadrant crossing, use this field to select the maximum number of degrees allowable for each circular block, regardless of quadrant crossings. Equivalent postprocessor commands:
PLABEL/OPTION,93,TO,90 $$ Maximum degrees per block=90
PLABEL/OPTION,93,TO,180 $$ Maximum degrees per block=180
PLABEL/OPTION,93,TO,270 $$ Maximum degrees per block=270
PLABEL/OPTION,93,TO,360 $$ Maximum degrees per block=360
NOTE: This option is also tied to the Quadrant Crossings default feature. Equivalent postprocessor commands for the same PLABEL/OPTION can be observed on that feature's help screen. More help is available for PLABEL 93.
This option is used for the handling the last point in a circular motion record if it falls outside of the true arc of the circle. Many toolpath generating systems use an iterative method for producing the toolpath for circular tool motion. In such cases a record is passed to the postprocessor indicating the following motion records are to be used for machining a radius or circle. If the tolerance band is sufficiently large it is possible that the last calculated point is outside the calculated arc of the radius or circle. This option provides several methods for handling these cases. Equivalent postprocessor commands:
PLABEL/OPTION,49,TO,0 $$ Do not correct for last CL point not being on true arc (default).
PLABEL/OPTION,49,TO,1 $$ Output linear move if last CL point is not on true arc.
PLABEL/OPTION,49,TO,2 $$ Make correction to radius, skipping linear move at end.
Enter the maximum radius allowed for circular interpolation. When the radius exceeds the value you enter here, the postprocessor generates linear moves to cut the circle.
Specify the z axis tolerance for analyzing the circle. If the Z deviation is greater that the specified value G1 helical interpolation will be output.
This option controls whether true radial feedrate calculations are used for circular interpolation. During circular interpolation, the velocity of the cutting edge of the tool is not the same as the velocity of the center of the tool radius. For example, a .20 tool radius driven around a .005 corner at 10 IPM would actually result in a tangential velocity of much less than 10 IPM. This option directs the postprocessor to adjust programmed feedrates to correct this condition. CAUTION:The caveat here is that adjustment of tangential feedrate can cause extremely high feedrate calculations under conditions where the cutter is large and the toolpath addresses small outside radii. Equivalent postprocessor commands:
PLABEL/OPTION,29,TO,0 $$ Do not adjust feedrate for circles (default).
PLABEL/OPTION,29,TO,1 $$ Adjust feedrate for circles.
Some controllers require that the register containing the radius be output on each circular interpolation block. Others retain the current value as modal. Modal codes are output only when their values change, not on every block. Check this box if the radius register is modal.
Some controllers require that the feed rate F-code be output on each circular interpolation block (G02/G03) even though it may be redundant. If you need this redundant F-code output with each circular interpolation (G02/G03) block, check this box. Note: This option only works with quadrant crossing output.
--------------------------------------------------------------------------------------------------------------------------
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