What's new
What's new
By:
Advanced search…

G72 Cuts more than programed

K

KevinEwards

Plastic
Joined
Aug 15, 2018
Hey I can't find any one with this problem. I was working on a part and using my Doosan Lynx 220 Turning center. Graphed before running the part. The machine wants to cut .030 more than I programmed.

M00;
;
;
T101;
G50 S3000;
G96 S500 M03;
G00 G54 G42 X2.3 Z0.25;
M08;
G72 W0.05 R0.01 (0.05 IS TO SEED UP SIM);
G72 P05 Q09 U0.0 W0.0 F0.002;
N05 G01 X2.3 Z0.0;
Z0.0;
N09 X-0.033;
;
;

The last cut is Z-0.030 when it should be Z0.0
Many thanks in advanc.
 
Probably your cutter comp G42. Try it without.


When i run a G72 it would look like this:
T101;
G50 S3000;
G96 S500 M03;
G00 G54 G40 X2.3 Z0.25;
M08;
G72 W0.05 R0.01 (0.05 IS TO SEED UP SIM);
G72 P05 Q09 F0.002;
N05 G0 Z0.0;
N09 G1 X-0.033;
 
I'm pretty sure the G42 needs to be in the G72 cycle on the N05 line.
Even though the G72 doesn't read the G42 INSIDE the P and Q lines, the G70 will. And since you have it turned on before the cycle, that might be where your .03 is coming from... assuming you have .03 in your comp.
 
Hazzert, I used FingerCAM and I have tip 3 with a 0.015 R in tool geometry
Tom the G72 was an after thought. I am still learning G-Code at tech and thought a G71 could handle the whole thing.
I'll try turning off TNRC.
 
KevinEwards said:
Hey I can't find any one with this problem. I was working on a part and using my Doosan Lynx 220 Turning center. Graphed before running the part. The machine wants to cut .030 more than I programmed.

M00;
;
;
T101;
G50 S3000;
G96 S500 M03;
G00 G54 G42 X2.3 Z0.25;
M08;
G72 W0.05 R0.01 (0.05 IS TO SEED UP SIM);
G72 P05 Q09 U0.0 W0.0 F0.002;
N05 G01 X2.3 Z0.0;
Z0.0;
N09 X-0.033;
;
;

The last cut is Z-0.030 when it should be Z0.0
Many thanks in advanc.
Click to expand...

Hello Kevin,

1. As Tom points out, there is no need whatsoever in using TNR Comp on a Face Cut that is perpendicular to the Z axis.

2. The tool is to the Left of the Tool Path in the direction it travels, accordingly, G41 should be used, not G42; that is the reason for your over-cut.

Regards,

Bill
 
You must log in or register to reply here.








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top