Haas lathe G71/G42/M0

brokenrinker · Dec 9, 2020

Using a G71 roughing cycle followed by G70 finish cycle. The tool path uses G42 compensation and ramps off (G40 with a X and Z move) after the "Q" block.
I've got a program stop after the ramp off so I can check dimensions prior to the finish cut. The control keeps saying I can't use a program stop with cutter comp engaged? Comp should have been turned off?

DouglasJRizzo · Dec 9, 2020

It probably wants a G40 move directly off the part in a linear move.

SeymourDumore · Dec 9, 2020

God! I'd like to wring the neck of the person that thought of the G70!
What? Third, perhaps fourth post just in the last couple of weeks about G70 problems?

DON'T FUCKING USE G70!
It's just a lazy way to program a garbage toolpath!
You either make an overcomplicated roughing path, or an underdefined finish path. Anything in-between sucks even more!

With that rant out of the way, post your code so we understand what you're trying to say by "after ramp-off".

yardbird · Dec 10, 2020

brokenrinker said:
Using a G71 roughing cycle followed by G70 finish cycle. The tool path uses G42 compensation and ramps off (G40 with a X and Z move) after the "Q" block.
I've got a program stop after the ramp off so I can check dimensions prior to the finish cut. The control keeps saying I can't use a program stop with cutter comp engaged? Comp should have been turned off?

Try putting the G42 down on the G70 line. You may have to start the spindle again after the M0. It's odd you want to measure before the finish runs, most times you measure afterwards then tweak size, rerun just the finish portion?

Brent

brokenrinker · Dec 10, 2020

This is an abridged version of what wont work.
T101
G54
G50 S2500
G97 S320 M03
G00 Z0.1
X2.76
G96 S200
M08
G71 P12 Q25 D0.03 U0.01 W0.01 F0.005
N12 G42 G00 X0 F0.01
G01 Z0. (origin)
X0.63 (1)
X0.75 Z-0.06 (2)
Z-0.625 (3)
X1.25 Z-1.875 (4)
X1.35 (6)
G03 X1.75 Z-2.075 R0.2 (7)
G01 Z-2.875 (8)
N25 X2.5
G40 X2.76
G00 Z0.1
M09
M00
G50 S2500
G97 S320 M03
G00 Z0.1
X2.76
M08
G96 S250
G70 P12 Q25
G40 G00 X2.76
Z0.1
M09

yardbird · Dec 10, 2020

Take the G42 from the N12 line and put on G70 P12 Q25 line?

Brent

Booze Daily · Dec 10, 2020

I would move N25 to the line with the G40. Might not work, but it keeps comp on and comp off within the profile. Neater code this way.

SeymourDumore · Dec 10, 2020

Remember: Your G70 ( yukk) code executes only between blocks N12 and N25.
Since your G40 code is after block N25, it will never execute when called by G70 (yukk)

You should change to this:
G01 X2.5
N25 G01 G40 X2.76

Ohh.. and ....aaaa.... ohhh .... Don't use G70!

Search

Largest Manufacturing Technology Community on the Web

Search

Haas lathe G71/G42/M0

brokenrinker

Plastic

DouglasJRizzo

Titanium

SeymourDumore

Diamond

yardbird

Titanium

brokenrinker

Plastic

yardbird

Titanium

Booze Daily

Titanium

SeymourDumore

Diamond

Similar threads