G71 for Stock Removal

[stuby]

Hello. I have a leadwell LTC-15 with a Fanuc-OT controller. I have used G71 for roughing and G70 to finish in the past, and it has worked well. Now, I am trying to do the same thing, using G71 for Stock Removal in Turning. I enter all of my G-codes, and everytime it begins the cycle, it feeds down to the final cut of the rough ( .01 on Dia, and .005 on faces still remains ) immediately, instead of doing the usual Linear cut. Here is my Code :

G01 Z0.1 X3.8
G71 U0.02 R0.1
G71 P1 Q2 U0.01 W0.005 F0.008
N1 G01
X1.15
G03 X1.25 Z-0.05 R0.05
G01 Z-.425
G02 X1.35 Z-.475 R0.05
G01 X2.90
G03 X3.0 Z-0.525 R0.05
N2 G01 Z-1.41

Thanks for the help, I hope I can figure this out...

[extanker59]

Isn't there suposed to be a rapid move between the N1 line and the first feed?
Like maybe:
G01 Z0.1 X3.8
G71 U0.02 R0.1
G71 P1 Q2 U0.01 W0.005 F0.008
N1 G0 X1.15
G1 Z0
G03 X1.25 Z-0.05 R0.05
G01 Z-.425
G02 X1.35 Z-.475 R0.05
G01 X2.90
G03 X3.0 Z-0.525 R0.05
N2 G01 Z-1.41

It's been a couple of years so I may be way off.

[CNCRim]

Originally Posted by stuby Hello. I have a leadwell LTC-15 with a Fanuc-OT controller. I have used G71 for roughing and G70 to finish in the past, and it has worked well. Now, I am trying to do the same thing, using G71 for Stock Removal in Turning. I enter all of my G-codes, and everytime it begins the cycle, it feeds down to the final cut of the rough ( .01 on Dia, and .005 on faces still remains ) immediately, instead of doing the usual Linear cut. Here is my Code : G01 Z0.1 X3.8 G71 U0.02 R0.1 G71 P1 Q2 U0.01 W0.005 F0.008 N1 G01 X1.15 G03 X1.25 Z-0.05 R0.05 G01 Z-.425 G02 X1.35 Z-.475 R0.05 G01 X2.90 G03 X3.0 Z-0.525 R0.05 N2 G01 Z-1.41 Thanks for the help, I hope I can figure this out...

Try this somehow your program doesn't work right. I think because N1 mess up.
G00 Z0.1 X3.8
G71 U0.02 R0.1
G71 P1 Q2 U0.01 W0.005 F0.008
N1 G0X1.15
G01Z0
G03 X1.25 Z-0.05 R0.05
G01 Z-.425
G02 X1.35 Z-.475 R0.05
G01 X2.90
G03 X3.0 Z-0.525 R0.05
N2 G01 Z-1.41

[dcoupar]

It's my understanding that N2 should be an X move back to the starting X. It's never failed when I've done it that way.

G01 Z0.1 X3.8
G71 U0.02 R0.1
G71 P1 Q2 U0.01 W0.005 F0.008
N1 G0 X1.15
G1 Z0
G03 X1.25 Z-0.05 R0.05
G01 Z-.425
G02 X1.35 Z-.475 R0.05
G01 X2.90
G03 X3.0 Z-0.525 R0.05
G01 Z-1.41
N2 G00 X3.8

[adamant]

Here is how I would do it.

G0 X3.8 Z.1
G71 U0.02 R0.1
G71 P1 Q2 U0.01 W0.005 F0.008
N1G0X1.15
G01Z0F.002
G03 X1.25 Z-0.05 R0.05
G01 Z-.425
G02 X1.35 Z-.475 R0.05
G01 X2.90
G03 X3.0 Z-0.525 R0.05
G1 Z-1.41
X3.8F.01
N2G0Z.1
G70P1Q2

Push the green button

[g-codeguy]

Originally Posted by stuby Hello. I have a leadwell LTC-15 with a Fanuc-OT controller. I have used G71 for roughing and G70 to finish in the past, and it has worked well. Now, I am trying to do the same thing, using G71 for Stock Removal in Turning. I enter all of my G-codes, and everytime it begins the cycle, it feeds down to the final cut of the rough ( .01 on Dia, and .005 on faces still remains ) immediately, instead of doing the usual Linear cut. Here is my Code : G01 Z0.1 X3.8 G71 U0.02 R0.1 G71 P1 Q2 U0.01 W0.005 F0.008 N1 G01 X1.15 G03 X1.25 Z-0.05 R0.05 G01 Z-.425 G02 X1.35 Z-.475 R0.05 G01 X2.90 G03 X3.0 Z-0.525 R0.05 N2 G01 Z-1.41 Thanks for the help, I hope I can figure this out...

N1 needs to have an X value. Out of about 25 lathes in our shop that can use this cycle, all but one will run with a G1 in the first block. That one lathe has to have a G0. Probably a parameter. Otherwise your program is fine...with one exception. Why are you retracting so far? My standard is R.01. You're wasting a lot of time cutting air.

You do not need to finish the cycle with an X3.8 unless you want the shoulder to be smooth. I personally wouldn't use a G0 if you did want to.

Using a G0Z.1 in the last block is redundant as the canned cycle will automatically rapid to X3.8Z.1 after it finishes.

What are you machining that the DOCs are so small?

[adamant]

Originally Posted by g-codeguy Using a G0Z.1 in the last block is redundant as the canned cycle will automatically rapid to X3.8Z.1 after it finishes.

Hey g-codeguy.

I realize that goz.1 in the qnline is redundant.......

The onley reason I do it is because the guy that tought me on a Hardinge conquest T42 is because he said that not all can cycles on all machines act the same and it is best just to be safe?

My guess is that that you have never seen a machine that did not retract in the can cycle?

So do you always end your QNline with the stock diameter in x?

Thanks
adamant

[ac123]

iv worked on a ltc 15, im in work tomoro morning ive got all the g codes still.
i think of the top of my head its on one line

G71P10Q20U.01W.002D200F.004

Note D this is your depth of cut.
then G70P10Q2O for finishing cut.

ill check tomoro at work.

[g-codeguy]

Originally Posted by adamant Hey g-codeguy. I realize that goz.1 in the qnline is redundant....... The onley reason I do it is because the guy that tought me on a Hardinge conquest T42 is because he said that not all can cycles on all machines act the same and it is best just to be safe? My guess is that that you have never seen a machine that did not retract in the can cycle? So do you always end your QNline with the stock diameter in x? Thanks adamant

Nope. Never ran a lathe in 23 years that didn't return to the canned cycle's starting position. That includes an Ikegai, and some Warner & Swaseys that were undoubtedly older than that when I started. Doesn't mean that there couldn't be some out there that don't, tho. I'm only familiar with Hardinge, Mori Seiki, Daewoo, Takisawa, Nakamura-Tome, Hitachi Seiki, Okuma, Yang, CMS, & some converted manual Hardinges with Fagor controls. Lot more brands out there.

As to ending the cycle at stock diameter...sometimes yes, sometimes no. Depends on where the cycle is ending.

BTW, I was only trying to point out that the Z.1 was unnecessary (to the best of my knowledge), not trying to take a dig at you. Or anyone else for that matter.

I try to keep my programs as clean as possible with no extraneous code. Naturally I ass-u-me that everyone else does also. Tain't necessarily true. Witness some programs with a G1 or G0 on almost every line. Now I suppose you are going to tell me that some lathes require it. You could be right.

[bbrreid]

ac123 has the answer you missed out the D for depth of cut on each pass

[g-codeguy]

Originally Posted by bbrreid ac123 has the answer you missed out the D for depth of cut on each pass

Never seen a G71 two block call that used a D code. The U.02 in the first G71 block is the depth of cut for each roughing pass.

A single block G71 call is something else.

[swarfmaker]

Hi Stuby,
code looks fine to me, are you sure you've not got another N1 or N2 line number any where in programme.
Regards