[Angus]

I am trying to cut a slot .672" wide along the X-Axis of a block, using a cutter of .500" diameter. Would someone mind looking at the following code and commenting on why the actual slot width would be .580". This is the first program that we have written for the Fadal VMC-20 that we just purchased, I can't figure out whether the program is incorrect, or we're doing somehting wrong in the set-up at the control. (Control is Fadal CNC88). Thanks for your help!

N84 M6 T3 D3 (.500 DIA X 4 FLUTE ENDMILL)
N85 (FINISH SLOT)
N86 (STEP NUMBER 50)
N87 M1
N88 G0 G17 G40 G80 G90
N89 M3 M8 S1528
N90 G54 X-0.3 Y0.714
N91 G43 H3 Z1.0
N92 Z0.1
N93 G1 Z-0.25 F18.3
N94 G41 Y0.664
N95 X3.78
N96 Y0.836
N97 X-0.3
N98 G0 G40 D0 Z0.1
N99 Z1.0
N100 G40 M5 M9

[ger21]

I think you need a lead in move for the offset to be applied. You might want to read this. http://65.204.160.42/fileadmin/fadal...ct_9_-_CRC.pdf

[Torsten]

You have programmmed a slot from x-.03 to x3.78
starting at y0.664 steping over to y0.836 that is a 0.172 stepdistance.
with a 0.5 diam. cutter should result in a 0.672 wide slot.
I assume there is a incorrect Tool offset value defined in
the D3 offset register.
Check this register and ensure the value there is zero.
Good Luck

[Angus]

You have programmmed a slot from x-.03 to x3.78
starting at y0.664 steping over to y0.836 that is a 0.172 stepdistance.
with a 0.5 diam. cutter should result in a 0.672 wide slot.
I assume there is a incorrect Tool offset value defined in
the D3 offset register.
Check this register and ensure the value there is zero.
Good Luck

Thakns for your reply. I appreciate the help. Question - when using G41, should I expect to see the coords for the center of the tool, or for the profile of the part?

[ger21]

Profile of the part.

[DareBee]

Your program looks correct, it is most likely in your MC tooltable. You could try substituting the D3 for H3. If you don't need tool offsets settable at the MC control the "H" will only use the tool heights from the table and ignore the other data.

[Brian J]

Might try moving your cutter comp offset from your toolcall line to the G43 H3 D3 or G41 D3. This is how we usually initiate cutter comp on our Fadals in format 2.

[pmurray]

After taking a quick glance, I too don’t see anything wrong the program. And if your tool wear settings look correct then I would look elsewhere for the problem.

First I would remove the G43 command (don’t use cutter comp) to simplify things. Without the cutter comp you should not be off by more than a few thousandths.

The difference between the width you’re getting and what it should be is almost .10”. Have you double checked the size of the endmill you are using?

plm

[gibbsman]

DO NOT remove the G43 line unless you want to bury a tool into the vise. The code looks okay except mabey try putting the 'D3' on line N94 after the G41.

[HuFlungDung]

For full tool radius comp, the profile should be the final profile. You have programmed an offset path, which basically does not require comp.
I backplotted your code, then offset the result to give what I think is the full size of the slot as it would be drawn. Then, I generated the following code. Your D3 value will be .5 to start:
T3 M06 ( 2FL SMT 1/2" CARB REG LEN 1.0")
G90 G80 G40 G54
G43 H3
S7500 M03
M08
G00 X-0.54 Y0.7602 Z0.2
Z0.05
G01 Z-0.25 F24.
G41 D3 X-0.55 F48.
Y0.414
X4.03
Y1.086
X-0.55
Y0.7602
G40 X-0.54
G00 Z0.2
M09
M01
M5
G00 G49 Z0.
G00 G53 X-20. Y0.
/T1 M06
M30