L32 G76 threading cycle

[Billcar2006]

I have just started program this machine. I am doing a g76 thread cycle but haven't got the manual I have G76 P010060. I know what the 3 values usually do, but I seem to be able to put 00 - 04 in for the the second set of digits. If I put anything else in the machine throws up a chamfer error. I thought I could put 15 in there and that's 1. 5 multiplied by pitch or does this cycle work different on citizen machines.

 

[TeachMePlease]

What control, it makes a difference.

For a Citizen with a Meldas it's a 2 line G76

G76P(# Cutting Passes, 00-99)(Chamfer amount 00-99)(Thread Angle 00-99) Q(Minimum Cut Depth) R(Finish pass amount)
G76 X/U(final diameter) Z/W(final length) R(taper height in radius, can be 0 for straight thread) P(thread height in radius) Q(first cut depth) F(thread lead)


So

G76 P101560 R.005
G76 U-.040 W.400 R0 P.020 Q .004 F.050

Would give you a thread that is cut in 10 passes, with a chamfer of 1.5 your lead, with a 60 degree thread form (first line)
It would cut a total of .040" on diameter (.020" per side) for a length of .400" in X, with 0 taper, .020" thread height (radial), first cut depth would be .004" and your feedrate is .050" per revolution.

Hope that helps.

If it's a FANUC.... Ignore me, cuz I gots no clue.

 

[Billcar2006]

What control, it makes a difference.

For a Citizen with a Meldas it's a 2 line G76

G76P(# Cutting Passes, 00-99)(Chamfer amount 00-99)(Thread Angle 00-99) Q(Minimum Cut Depth) R(Finish pass amount)
G76 X/U(final diameter) Z/W(final length) R(taper height in radius, can be 0 for straight thread) P(thread height in radius) Q(first cut depth) F(thread lead)


So

G76 P101560 R.005
G76 U-.040 W.400 R0 P.020 Q .004 F.050

Would give you a thread that is cut in 10 passes, with a chamfer of 1.5 your lead, with a 60 degree thread form (first line)
It would cut a total of .040" on diameter (.020" per side) for a length of .400" in X, with 0 taper, .020" thread height (radial), first cut depth would be .004" and your feedrate is .050" per revolution.

Hope that helps.

If it's a FANUC.... Ignore me, cuz I gots no clue.

It's a meldas 600 controller. I have the g76 on 2 lines. What I'm trying to find out is on the first line the second 2 digit in the p value it will only let me put in 00, 01, 02, 03 or 04 for the chamfer. Anything else it throws up a chamfer alarm. I want to know what these values equate to.

 

[TeachMePlease]

Post your whole code. And the exact alarm.

 

[angelw]

What I'm trying to find out is on the first line the second 2 digit in the p value it will only let me put in 00, 01, 02, 03 or 04 for the chamfer. Anything else it throws up a chamfer alarm. I want to know what these values equate to.

Hello Bill,
Welcome to the Board and may I say, what a great name you have.

The second two digits of the "P" address is the chamfer amount at the finish end of the Thread, in units of 0.1 x L (where L = Thread Lead), designated by a two digit Integer in the range 0.0 to 9.9 without a decimal point. Its unusual that you can only specify 00 to 04.

As suggested by TeachMePlease, Post a copy of the section of your program under discussion.

Regards,

Bill