Programming #CYL [EDGES..]
Notice
The kinematic parameters in ID 79 must be set for this machining type.
Syntax to select profiled tube machining:
Syntax: | |
#CYL [ EDGES=.. ROUNDING=.. LENGTH1=.. [LENGTH2=.. ] | modal |
EDGES=.. | Number of edges (corners) of the profiled tube, positive integer The minimum number of corners on the profile is limited to 3 and the maximum number to 16. |
ROUNDING=.. | Edge rounding radius (corner radius), [mm, inch]. |
LENGTH1=.. | Side length for symmetrical tubes or first side length for rectangular tubes, [mm, inch] |
LENGTH2=.. | Second side length for rectangular tubes, [mm, inch] |
VEL=.. | Path velocity on edge rounding [mm/min] |
ACC=.. | Path acceleration on edge rounding [mm/min2] |
Syntax to deselect profiled tube machining:
Syntax: | |
#CYL OFF | modal |
Programing Example
#CYL [EDGES..]
(Symmetrical square profile with 100 mm edge length)
(and 10 mm edge rounding radius)
N10 #CYL [EDGES=4 ROUNDING=10 LENGTH1=100]
...
(Asymmetrical square profile with edge lengths of 100 mm)
(and 80 mm and 15 mm edge rounding radius)
N10 #CYL [EDGES=4 ROUNDING=15 LENGTH1=100 LENGTH2=80]
...
(Reduced path dynamics on the profile rounding)
N10 #CYL [EDGES=4 ROUNDING=5 LENGTH1=50 LENGTH2=50
ACC=1000000]
Attention
With relative programming, the number of profile rotations is limited for each block due to resources. An error message is generated if the maximum number is exceeded.
Programing Example
Tube profile machining
(* Tube profile machining *)
%main
N10 #SLOPE [TYPE=STEP]
N20 G90 X0 Y0 Z100 U0
N30 U0 X0
N40 #CYL[EDGES=4 ROUNDING=5 LENGTH1=20 LENGTH2=20]
N50 G01 G91 X10 F5000
N60 U50
N70 G03 U-100 I300 J-50
N80 #CYL OFF
N90 M30
Rectangular profile
Activation condition
Default case: Selecting on plane surface
The transformation is selected when the workpiece is aligned flat. The angle of the U axis then displayed with horizontal workpiece alignment is set by means of a U offset (kinematic parameters).
When #CYL[..] is selected, the Y axis position of the tool is located within the plane surface of the workpiece (side length LENGTH1), otherwise an error message is output.
Special case: Selection on profile rounding
A U angle offset may possibly have to be set in the same way as described before.
The transformation should be selected on the profile rounding. This variant can be used when machining was stopped with active transformation on the profile rounding or a profile rounding position was approached using #PTP ON. The CNC checks whether selection is possible with the current active U and Y axis positions. An error message is generated if an axis position are invalid.
Notice
With G90 absolute programming, positioning on the circumference is always based on the "shortest path” without specifying the direction of rotation.
Please note the section "Programming modulo axes" in [PROG] when programming the sign for the direction of rotation.
This must also be taken into account for circular motion blocks (G02, G03) with absolute target point programming.