If you have found the D register for tool radius in your Mach controller (which I know nothing about, btw), you would typically enter the nominal tool radius (or diameter depending on what Mach expects you to use).
You may have to wait for someone to come along who uses Dolphin, to figure out just how you are supposed to get it to post a machine radius compensation correctly.
Here is a small program you can do a test run with. It is based on a 2" square, with 1/8" radius corners. This is how it could look, although the start point and end point are totally up to the user to pick, I took no pains about where I began.
T1 M06 ( 4FL SMT 1/4" CARB REG LEN .75")
G90 G80 G40
G54
/G00 X0 Y0
G43 H1
S5000 M03
M08
G00 X1.675 Y0.9042 Z1.
X1.675 Y0.9042 Z0.05
G01 S5000 X1.675 Y0.9042 Z-0.05 F12.
G41 D1 X1.775 Y0.7792 F24.
G03 X2. Y1.0042 I0. J0.225
G01 X2. Y1.875
G03 X1.875 Y2. I-0.125 J0.
G01 X0.125 Y2.
G03 X0. Y1.875 I0. J-0.125
G01 X0. Y0.125
G03 X0.125 Y0. I0.125 J0.
G01 X1.875 Y0.
G03 X2. Y0.125 I0. J0.125
G01 X2. Y1.0042
G03 X1.775 Y1.2292 I-0.225 J0.
G01 G40 X1.675 Y1.1042 Z-0.05
G00 X1.675 Y1.1042 Z1.
M09
M01
M5
G00 G91 G28 Z0
G00 G90 G53 X-20. Y0.
T1 M06
M30
__________________
First you get good, then you get fast. Then grouchiness sets in.
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management) |