G78 Threading cycle Hurco TM6

[Dupa3872]

Guy's,

I have another thread, Ha Ha up about this machine and this cycle but it may have run it's course so I'm starting fresh with another.

I bought two identical Hurco TM6 CNC lathes. We only program our work in Master Cam and will not be using the Hurco's programing side. Turns out one of the machines will only thread using a G78 cycle witch I am told is similar to the Fanuc G76 cycle.

Other than standard drill cycles we do not use canned cycles and are a bit lost using this G78. If you have a Hurco and use G78 for O.D. and I.D. threads I would be grateful if you would post a copy of your code for a 5/8-20 OD thread and perhaps one for an ID thread.

We have been messing around losing valuable time on jobs for a few days now and really need some help.

Thanks

Ron

This is the sample we have been trying to tweak to work on a 5/8-20 thread by changing the numbers. This sample is Metric and some of the numbers don't make sense to us.

G78 Threading Cycle Format

G78 P010060 Q100 R0.05
G78 X30 Z-20 P1024 Q200 F2

First block of the G78 Threading cycle

G78 : G code for threading cycle.

P : P actually consists of multiple values which control the thread behavior,

01 : Number of spring passes or spring cuts or finishing cuts.
00 : Thread run out.
60 : Flank angle or Infeed angle (allowed values 0, 29, 30, 56, 60, 80).

Q : Depth of cut.
R : Depth of Finish cut

Second block of the G78 Threading cycle

G78 : G code of the threading cycle.
X (U) : The end value in x-axis.
Z (W) : The end value in z-axis.
P : Thread depth ( as radius value ).
Q : Depth of first cut.
F : Thread Pitch
R : Thread Taper

N17 T101
N18 G54
N19 G97 S800 M3
N20 G0 X32 Z6 M8
N21 G76 P010060 Q100 R0.02
N22 G76 X28.161 Z-50 P919 Q250 F1.5
N23 G0 X150 Z100

 

[awander]

I don't know anything about Hurco or G78, but is a 60 degree infeed angle (as shown in your code) correct?

 

[angelw]

Guy's,

I have another thread, Ha Ha up about this machine and this cycle but it may have run it's course so I'm starting fresh with another.

I bought two identical Hurco TM6 CNC lathes. We only program our work in Master Cam and will not be using the Hurco's programing side. Turns out one of the machines will only thread using a G78 cycle witch I am told is similar to the Fanuc G76 cycle.

Other than standard drill cycles we do not use canned cycles and are a bit lost using this G78. If you have a Hurco and use G78 for O.D. and I.D. threads I would be grateful if you would post a copy of your code for a 5/8-20 OD thread and perhaps one for an ID thread.

We have been messing around losing valuable time on jobs for a few days now and really need some help.

Thanks

Ron

This is the sample we have been trying to tweak to work on a 5/8-20 thread by changing the numbers. This sample is Metric and some of the numbers don't make sense to us.

G78 Threading Cycle Format

G78 P010060 Q100 R0.05
G78 X30 Z-20 P1024 Q200 F2

First block of the G78 Threading cycle

G78 : G code for threading cycle.

P : P actually consists of multiple values which control the thread behavior,

01 : Number of spring passes or spring cuts or finishing cuts.
00 : Thread run out.
60 : Flank angle or Infeed angle (allowed values 0, 29, 30, 56, 60, 80).

Q : Depth of cut.
R : Depth of Finish cut

Second block of the G78 Threading cycle

G78 : G code of the threading cycle.
X (U) : The end value in x-axis.
Z (W) : The end value in z-axis.
P : Thread depth ( as radius value ).
Q : Depth of first cut.
F : Thread Pitch
R : Thread Taper

N17 T101
N18 G54
N19 G97 S800 M3
N20 G0 X32 Z6 M8
N21 G76 P010060 Q100 R0.02
N22 G76 X28.161 Z-50 P919 Q250 F1.5
N23 G0 X150 Z100

Hello Ron,
Not one thing in your example program was anywhere near the Thread you wanted to cut (5/8 x 20TPI), not even the Lead.

Q : Minimum Depth of cut.
R : Depth of Finish cut

G78 : G code of the threading cycle.
X (U) : The end value in x-axis.
Z (W) : The end value in z-axis.
P : Thread depth ( as radius value ).
Q : Depth of first cut.
F : Thread Pitch
R : Thread Taper

Following is code that will be close to what you want to cut a 5/8 x 20 TPI, External Thread.

N17 T101
N18 G54
N19 G97 S1200 M3
N20 G0 X18.0 Z6 M8
N21 G76 P010060 Q100 R0.02
N22 G76 X14.363 Z-50 P756 Q500 F1.27
N23 G0 X150.0 Z100.0

Regards,

Bill

 

[Dupa3872]

Hello Ron,
Not one thing in your example program was anywhere near the Thread you wanted to cut (5/8 x 20TPI), not even the Lead.

Q : Minimum Depth of cut.
R : Depth of Finish cut

G78 : G code of the threading cycle.
X (U) : The end value in x-axis.
Z (W) : The end value in z-axis.
P : Thread depth ( as radius value ).
Q : Depth of first cut.
F : Thread Pitch
R : Thread Taper

Following is code that will be close to what you want to cut a 5/8 x 20 TPI, External Thread.

N17 T101
N18 G54
N19 G97 S1200 M3
N20 G0 X18.0 Z6 M8
N21 G76 P010060 Q100 R0.02
N22 G76 X14.363 Z-50 P756 Q500 F1.27
N23 G0 X150.0 Z100.0

Regards,

Bill

Thanks Bill that's a big help. That was not the code for the thread we were trying to make. That code came from an example I found on the Hurco web site. I should have posted our code and then it would have been clear where we were going wrong. I think what you posted will go a long way and get us making chips.

Thanks You !!

Make Chips Boys !

Ron

 

[Dupa3872]

I don't know anything about Hurco or G78, but is a 60 degree infeed angle (as shown in your code) correct?

Hi,

That was not the code for the thread we were trying to make. That code came from an example I found on the Hurco web site. I do not usually use an in feed angle at all when I program threads. I should have posted our code.

Thanks

Ron

 

[angelw]

I don't know anything about Hurco or G78, but is a 60 degree infeed angle (as shown in your code) correct?

Hello awander,
The angle specified in the Threading Cycle is the included angle of the Thread Form, or the Threading Insert. The control will use the specified angle dived by two as the In-feed. With a 60deg included angle, in practice, its better to specify 55degs as the included angle so that the trailing edge of the insert takes a small cut on the trailing thread flank. On thread with a large Thread Height, a noticeable stepped surface can result when the same angle as the included angle of the Threading Insert is specified.

Regards,

Bill

 

[awander]

Hello awander,
The angle specified in the Threading Cycle is the included angle of the Thread Form, or the Threading Insert. The control will use the specified angle dived by two as the In-feed. With a 60deg included angle, in practice, its better to specify 55degs as the included angle so that the trailing edge of the insert takes a small cut on the trailing thread flank. On thread with a large Thread Height, a noticeable stepped surface can result when the same angle as the included angle of the Threading Insert is specified.

Regards,

Bill

Thanks, Bill