FANUC G76 CYCLES

[BenzB]

Hello, we recently purchased a DMC mill turn lathe with a Fanuc Oi Tc/Mc control on it. Yesterday we were attempting to cut a thread (turning) using the G76 cycle. A couple of issues came up. One being that this machine uses a single line G76 cycle vs. double line G76 cycle. Is there a parameter that can be changed to switch this control to make use of the double line cycle?

 

And we also had an issue with the tool retracting (in X) from the thread before it reached the Z end point (about an inch shy) and then continued on to the Z end point before finally retracting from the bore. Any clues as to why it would do this? The code line looked fine.

 

Thanks

Benz

[jeff]

Yes this is usually a parameter switch.

[Guest MTB Technical Services]

Hello, we recently purchased a DMC mill turn lathe with a Fanuc Oi Tc/Mc control on it. Yesterday we were attempting to cut a thread (turning) using the G76 cycle. A couple of issues came up. One being that this machine uses a single line G76 cycle vs. double line G76 cycle. Is there a parameter that can be changed to switch this control to make use of the double line cycle?

 

And we also had an issue with the tool retracting (in X) from the thread before it reached the Z end point (about an inch shy) and then continued on to the Z end point before finally retracting from the bore. Any clues as to why it would do this? The code line looked fine.

 

Thanks

Benz

 

Yes, Parameter #1 BIt #1=0

 

Keep in mind that if you change this you may run into issues with other cycles because of it.

Typically, the machine tool builder sets up the machine with it's default format because of how they want the machine to handle certain cycles.

Changing this parameter will effect ALL cycles, not just G76.

 

What you can do is change the parameter dynamically.

The example below goes the opposite way, from double-ine to single and then back.

The P2 word indicates a staggered cycle that uses both sides of the insert.

 

 

The retraction you are getting is likely the chamfering amount so you don't ring the last thread.

Something is probably incorrect in your syntax.

 

If you post the code you actually tried to run, it would be easier to give you a more specific answer..

[BenzB]

Here is the code we ran:

G97 S50 M4;

G0 X2.275 Z.2 M8;

G76 X2.5395 Z-6.3 K1600 L0 D210 A0 P0 F1.0;

Z.2 M9;

 

The Z-6.3 should have been Z-5.3 but we had to cheat it because of the retraction.

 

Thanks for the help!

[Guest MTB Technical Services]

Here is the code we ran:

G97 S50 M4;

G0 X2.275 Z.2 M8;

G76 X2.5395 Z-6.3 K1600 L0 D210 A0 P0 F1.0;

Z.2 M9;

 

The Z-6.3 should have been Z-5.3 but we had to cheat it because of the retraction.

 

Thanks for the help!

 

 

What thread are you actually trying to cut?

Your feedrate value looks odd in that it appears to not be an IPR value that reflects the thread pitch.

 

Additionally, the cycle code is not correct.

The L address really doesn't need to be used.

However, if it is used, it can't be zero.

L = Total Thread Length Travel

 

The A address really shouldn't be zero either.

That's the included angle of the insert infeed control.

There are only six permitted values.

Zero is a permitted value but I've always avoided it as it's a direct radial infeed.

 

The P address can't be zero either.

The values need to be P1, P2, P3 or P4.

 

P1 = Single face cutting with constant cutting amount.

P2 = Dual face cutting with constant cutting amount.

P3 = Single face cutting with constant cutting depth.

P4 = Dual face cutting with constant cutting depth.

 

You should refer to the user manual for the M-code that controls the chamfering exit.

 

This freeware utility I wrote should help.

http://www.mtbtech.net/blog/2013/10/01/Free-G76-Thread-Cycle-Generator.aspx

 

[BenzB]

It is actually a square form (.08" wide x .08" deep) lubrication groove on a 1" pitch left hand spiral in a bushing. I am using a 2mm wide top notch groover. All I can have is radial depth of cut changes..
Also, according to my manual, P0 is the same as P1.

I will try taking the L out to see if that fixes it.

 

[Guest MTB Technical Services]

It is actually a square form (.08" wide x .08" deep) lubrication groove on a 1" pitch left hand spiral in a bushing. I am using a 2mm wide top notch groover. All I can have is radial depth of cut changes..

Also, according to my manual, P0 is the same as P1.

I will try taking the L out to see if that fixes it.

G76 - 1 line.JPG

 

 

OK, I can see from your manual that you have an older machine.

Check your M-code list for M23 & M24 for retract of chamfering.

You'll have a pair of M-code that control this.

This controls your exiting of the thread so you don't ring it

 

Their description of the L address, or thread lead, can be confusing.

It's the axial travel for one 360 degree revolution.

Thread lead will change based on the number of starts.

If you have a 1-8 single start thread, the lead and the pitch are equal.

If you have a 1-8, 4 start thread,the lead is 0.5 per start.

Each start will by offset by 90 degrees of spindle rotation and the pitch in Z.

 

The pitch is still 0.125 on the final part.

It's easy to verify with the mating nut or rod as the number of starts must match.

 

The one thing you can't do is use both L and F.

It's one or the other.

In your case, you should eliminate it completely.

 

it's definitely the reason you are having issues with the Z.

Take it out.