[engM]

Hi, Thanks for the nice administrators Forum .
There are lots of useful information.
I write from Italy, for a problem ;

I have the following milling to be carried with G-code;

we have to work with the coordinates of the center of the cutter. D=40mm and r= 20

here is the program done in my possession;

T01 01 M6
G94 g97 s f
G00 X 73.535 Y 108.535 Z2
G01 X 73.535 Y 108.535 Z-4 (P1)
G02 -61.56 Y 106.42 Z-4 I -73.535 J 73.535 k-4 (P2)
G03 x 61.56 y 106.42 z-4 I 0 J275.56 k-4 (P3)

I'll stop here for now;
I ask you, Why P2 is used for the portion size x = 61.55 and y = 106.41 ???

and not X 73.535 Y 108.535 ?

thanks for any explanations, sorry for the bad English

[fordav11]

To work it out do the math. It's just some simple trigonometry.
You should be using G41/G42 etc

The correct code to profile around the outside of the R15/R200 shape is below.....

G0 X-135.0 Y73.525
Z5.0
G1 Z-4.0 F100.0
G1 G42 D1 X-88.525 Y73.525
G3 X-87.62 Y68.395 I15.0 J0
G2 X-87.62 Y-68.395 I-187.938 J-68.395
G3 X-68.395 Y-87.62 I14.095 J-5.13
G2 X68.395 Y-87.62 I68.395 J-187.938
G3 X87.62 Y-68.395 I5.13 J14.095
G2 X87.62 Y68.395 I187.938 J68.395
G3 X68.395 Y87.62 I-14.095 J5.13
G2 X-68.395 Y87.62 I-68.395 J187.938
G3 X-88.525 Y73.525 I-5.13 J-14.095
G1 G40 X-135.0
G0 Z100.0

[engM]

To work it out do the math. It's just some simple trigonometry.
You should be using G41/G42 etc

The correct code to profile around the outside of the R15/R200 shape is below.....

G0 X-135.0 Y73.525
Z5.0
G1 Z-4.0 F100.0
G1 G42 D1 X-88.525 Y73.525
G3 X-87.62 Y68.395 I15.0 J0
G2 X-87.62 Y-68.395 I-187.938 J-68.395
G3 X-68.395 Y-87.62 I14.095 J-5.13
G2 X68.395 Y-87.62 I68.395 J-187.938
G3 X87.62 Y-68.395 I5.13 J14.095
G2 X87.62 Y68.395 I187.938 J68.395
G3 X68.395 Y87.62 I-14.095 J5.13
G2 X-68.395 Y87.62 I-68.395 J187.938
G3 X-88.525 Y73.525 I-5.13 J-14.095
G1 G40 X-135.0
G0 Z100.0

thank you very much Fordav;




if you wish, you may also be programmed with the coordinates of the tool center

fore example;

-73.535- 15*cos(20°) = -87.62

-87.62 -(D/2) Cos(20°) = -106.41 = Coordinate x of center tool;

so the exercise becomes much more complicated ^^!


12.38- D/2 = 12.38

[fordav11]

I don't need an exercise. there's no point wasting time with more calculations than required.
program it using G41/G42, get the job done and move on.

the center section can be programmed to center coordinates but only because it is very simple to do using a 40mm diameter cutter.

[engM]

I don't need an exercise. there's no point wasting time with more calculations than required.
program it using G41/G42, get the job done and move on.

the center section can be programmed to center coordinates but only because it is very simple to do using a 40mm diameter cutter.

exactly;
the professor had requested the coordinates of the shear center, for the year;
really a loss of time.

thanks again and see you soon

[fordav11]

to program to center is just as easy as programming to the edge.
the outer profile is extended 20mm and R15/R200 becomes R35/R180.
the trigonometry is the same.
but using G41/G42 allows the program to have sizes that match the drawing and also allows easy adjustment with the diameter offset.
If you want a sloppy, poorly coded program using incorrect methods you need to talk to someone who has no idea about real machining or real CNC programming. i.e. ask your 'professor'.
alternatively work it out yourself using my program above as a base.