Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 433)

Using Chamfers and Corner Radius
Chapter 16
16-3
Example 16.2
Linear-to-Circular Motions with Chamfer
N10 G00 X0 Y0 F100;
N20 G01 X10. Y10., C3;
N30 G02 X20. Y20. R10;
N40 M30;
Figure 16.2
Results From Chamfer Example 16.2
Actual start point of
block N30 and end
point of chamfer block
Programmed end point
of block N20
Actual end point of block N20 and
start point of chamfer block
C
C (chord length)
N30
Chamfer
block
N20
25 20 15 10 5
20
15
10
5
Y
X
Corner Radius
Use the ,R command to program a radius between two intersecting tool
paths. The R command must be programmed after a comma (,). Program
the ,R followed by the radius size in the block where the first path is
programmed. The control looks ahead to the block commanding the
second path, and automatically inserts the circular rounding block to meet
that path. This inserted, circular block is always tangent to both
programmed tool paths. If the control cannot generate an arc that is
tangent to both paths with the programmed ,R , then the control will
generate an error.
The first corner radius block always terminates at the point on the block
where the rounding block is tangent to the first block. The rounding block
terminates at the point where the generated rounding block is tangent to the
second rounding block. The second rounding block starts from the
end-point of the generated circular block and continues on to the
programmed end-point of the second block.
Important: If the two motion blocks are tangent to each other, then any
corner-rounding commands are ignored.