how do u change infeed to alternating? we have a new part that we have to thread on a fanuc 18t control. or just a compound infeed is it the first line p011060 or is it some paramiter . any help would be apreciated
the rookie threader

What do you mean by alternate threading?
Do you want the infeed to alternate from front to back?
Some of the older, and way more expensive controls had this option, but I think you need to stick with the angle input that corrects the infeed for the angle you are calling out in the first line of the G76 as it goes deeper.
If you have other questions, look at the examples I have on my website.
www.doccnc.com
Heinz.

To do alternate flank infeed in the G76 cycle on a 0i , 18i ,21i control you have to use the old one line cycle format.

Example:

G76 X2.29 Z-1.0 K1560 D500 F.25 A60.P2

The P2 is the code that switcheds on alternate flank infeed.

K- Thread depth per side.
D- Depth of first cut
A- Included angle

Please let us know how it goes.

Regards
Deon

Are you sure you wouldn't have to set a parameter to be able to switch to the single-line G76 format?

My Fanuc book for the 18T control shows parameters in a range of 5130-5132 and 5140-5143 controlling much of the finer details of a G76 cycle. Unfortunately, I didn't have the inclination to spell it all out. Plus, I am not a good re-translator of Japanese to English. What they say in the book isn't always a clear picture of what the values in the parameters actually do. That's Fanuc-speak for you. Good luck.

As per 0i parameter manual, 0001#1 (FCV) selects between series 0 format (series 16/18 compatible format) and series 10/11 format. There are references to FS15, but it is not explained how to select this format. Any idea?

thanks , what i,m gathering is that the 2 line format gives u 6 infeed angles
only in one direction. that should be ok, i will try the one it calls out for the angle i need. i tried the 2 line format on the machine and seemed to
work ok. ( with out cutting a chip) i should be cutting chips soon tho

The following example of 2-block G76 would be helpful. It makes M30 thread of 30 mm length:

O0008
G21 G97 G98
G54
G28 U0 W0
T0707
M03 S200
G00 X32 Z10
G76 P031560 Q150 R0.15
G76 X25.706 Z-30 P2147 Q250 F3.5
G28 U0 W0
M05
M30

The threading cycle in this program is based on the following parameters:
Number of finishing passes = 3
Chamfer distance = 1.5 × 3.5 = 5.25 mm (3.5 mm is pitch)
Thread angle (tool-tip angle) = 60 degree
Minimum depth of cut = 150 micron = 0.15 mm
Finishing allowance (on dia.) = 0.15 mm
Core diameter = 25.706 mm (from threading chart)
Axial end of thread = 30 mm in the negative Z−direction
Depth of thread = 2147 micron = 2.147 mm (from threading chart)
First depth of cut = 250 micron = 0.25 mm
Lead (= pitch, for single-start) = 3.5 mm

There is also a provision for an R-word in the second block of G76 for taper threads.

Hi steelman,
I know that what you wants to know.

If you select 'P021560' threads goes to single side entering in threads profile.

If you select 'P021500' threads goes to streight entry like G92 code style.

If you select 'P021530' or P021529' threads goes to small zigzag type in z axis style.

If you select 'P021520' threads goes to another big zigzag type style.

You can change angles and see results.

This not only thread angle but can change style also.

Naval Chauhan