Need Fanuc threading help

[camaro_dan67]

My machine has a Fanuc 21i-t control. I am trying to thread a 3/8-24 external thread. I have a 24 tpi full profile insert.
This control is fairly new to me. My experience is threading on a haas lathe. On the haas my threading program would look something like this.

M98 P7000
T101 S1000 M03
G54
M08
G0 X.4 Z.1
G76 X.332 D.015 K.034 F.0416Z-.3
G0 X1.0
M98P1000
M30

Can somebody put that threading cycle in Fanuc terms and explain the variables and how they got them.
I do have a manual and it says not to use decimals for most of the variables. I have a cycle that makes a thread but it takes one very deep cut then one finish pass. Unfortunately I don't have the cycle I wrote in front of me.

 

[sinha]

Search for G76 on this forum. A lot of information is already available. No point in repeating the same thing again. Ask specific question if something is not clear.

Normally, 2-block G76 is used on Fanuc.

 

[DouglasJRizzo]

On newer Fanuc controls the threading is a two line cycle.
No offense, but your program is - to my eyes - not really right.
@sinha is correct, there are many G76 examples here on the site.

I'll add mine, even tho this has been covered before.

O1000(EXAMPLE)
G0 G40 G99 T0101
X4. Z4. M8
G97 S1000 M3 (NOTE)
X.625 Z.25 (NOTE)
G76 P020060 Q0020 R0020
G76 X.332 Z-.375 P0340 Q0020 F.0416
X4. Z4. M9
G28 U0
G28 W0 M5
M30
%

 

[camaro_dan67]

I ended up using a G78. Being that it was Teflon I am threading I also needed to program a little taper in the cycle.
Thanks everyone.

 

[sinha]

I ended up using a G78

Your machine is set to G-code system C.
System A uses G76.

 

[Ox]

 

[Fancuku]

Your machine is set to G-code system C.
System A uses G76.

Or it could be system B where G78 is the same as G92 in system A.

 

[camaro_dan67]

Ok thanks everyone. Looks like I have the information I need.

 

[sinha]

Or it could be system B where G78 is the same as G92 in system A.

That is correct, but G92 does not have too many arguments which he is using.

 

[SeymourDumore]

No offense, but your program is - to my eyes - not really right.

He posted a Haas single line G76 code, which is also accepted by Fanuc with some parameter change.
That said, you are correct that there are some questionable numbers there.

G0 X.4 Z.1
G76 X.332 D.015 K.034 F.0416Z-.3

Those in red should be X.322 and K.026

But then your post:

X.625 Z.25 (NOTE)
G76 P020060 Q0020 R0020
G76 X.332 Z-.375 P0340 Q0020 F.0416

What's up with the thread starting in Cambodia?

To the OP:

You can look up the full explanations of G76 on this board, should be dozens of them.
As for your need with a .001 taper added:

G76 P020060 Q0020 R0020
G76 X.322 Z-.3 P260 Q20 R-10 F.0416

Those in blue can't have decimals, the rest is OK with.

 

[sinha]

R-10

May be parameter dependent.

 

[DouglasJRizzo]

He posted a Haas single line G76 code, which is also accepted by Fanuc with some parameter change.
That said, you are correct that there are some questionable numbers there.

Yes, there could be a parameter change, but then on some new Fanuc controls, other features can be disabled when that happens. Not sure why.

G0 X.4 Z.1
G76 X.332 D.015 K.034 F.0416Z-.3

Those in red should be X.322 and K.026

I just used his data, however on two line Fanuc cycles, "K" isn't used, it's "P" for thread height. Also, the Z addy should be next to the X (just easier to read) and decimal points are not allowed for "P" and "D" addresses in Fanuc land.

But then your post:



What's up with the thread starting in Cambodia?

I always give .25" in X and Z when starting a thread cycle. If your initial D.O.C. and P are correct, it won't cut air and gives the control some room to work. I've seen people nip the tops of the threads off by starting too close in X and have a lousy start when too close in Z.

To the OP:

You can look up the full explanations of G76 on this board, should be dozens of them.
As for your need with a .001 taper added:

G76 P020060 Q0020 R0020
G76 X.322 Z-.3 P260 Q20 R-10 F.0416

Those in blue can't have decimals, the rest is OK with.

 

[sinha]

I've seen people nip the tops of the threads off by starting too close in X

The clearance in X must be at least k (height of thread) away from the top of thread, otherwise, the top of the thread might be nipped when feedhold is applied.

 

[Ox]

I always give .25" in X and Z when starting a thread cycle. If your initial D.O.C. and P are correct, it won't cut air and gives the control some room to work. I've seen people nip the tops of the threads off by starting too close in X and have a lousy start when too close in Z.

WOW!

A 1/4" in X?

I can appreciate not clipping the crests, but the more retract that you have in X, the longer your pull-out length will be.


-------------------

I am Ox and I approve this here post!

 

[EmGo]

decimal points are not allowed for "P" and "D" addresses in Fanuc land.

You guys and yer cycles. I'm gonna buy y'all a big box of kotex and ship it over, maybe that'll help

 

[DouglasJRizzo]

WOW!

A 1/4" in X?

I can appreciate not clipping the crests, but the more retract that you have in X, the longer your pull-out length will be.


-------------------

I am Ox and I approve this here post!

If it's coming straight out, it goes right to the X start point.
@EmGo does have a point. Using G32 or G92 would be much faster..

 

[Ox]

I see that you use Pxx00xx, so in your case it would not be an issue I guess.


--------------------

I am Ox and I approve this here post!

 

[sinha]

In angled retraction, the tool starts retracting radially, as it approaches the Z end. As a result, it has to cover a smaller distance to reach the start X, in the end. Therefore, straight pull out would take slightly more time. However, an extra distance of 2-3 mm at rapid rate hardly makes any difference.

 

[triumph406]

WOW!

A 1/4" in X?

I can appreciate not clipping the crests, but the more retract that you have in X, the longer your pull-out length will be.


-------------------

I am Ox and I approve this here post!

If your doing 20 parts, no big deal.

2000 parts, sure that's too much.

I'm in the very low part count end of the industry, I don't sweat too much if there's too much air being cut (at 25% rapid)

 

[Ox]

Nothing to doo with time, and everything to doo with pull-out length.

If you want threads close to a shoulder, you don't want the cross slide pulling out any earlier than needed.

If you are like Rizzo, and you run a "00" pull-out, then not an issue.
If you run an "01" or larger, then your X will start pulling out sooner - the more X that you tell it to move.

Maybe the rest of the world runs "00"? IDK...
I typically run an "01" - mostly just b/c I always have.
And I'm going to ass_u_me that the rest of you doo the same (as you normally do) on most jobs as well?

"00" just seems harsh to me.
I try to NOT use it unless absolutely sensinary.
???


-----------------------

I am Ox and I approve this here post!