threading trouble

[ZWM51]

Have a cnc lathe with fanuc o-t controller. Using a G76 threading cycle. I want to know how to controll first depth of cut and finshing depths of cut?

thanks,
zw

[dcoupar]

The depth of the first pass is controlled by Q in the 2nd G76 block. The minimum depth of cut is controlled by Q in the 1st G76 block.

[sinha_nsit]

... in microns (in mm mode)

[ZWM51]

in english or inchs

[sinha_nsit]

It is least input increment.
So, it would be number of steps of 0.0001 inches.

This reminds me of another issue:
mm mode is 2.5 times more accurate than inch mode, in terms of least input increment. In other words, the resolution is better in mm mode.

[ZWM51]

Still cant control depth of cut. Changed second Q still doesnt change depth of cut. Keeps breaking threading insert on first pass. We're trying to id thread M14X1.5 in carbon steel. Here is the program trying to use. Can somebody look at make sure its right or send me a program.

T0202
S100M3
G00X0.514
Z.1
G76 P030160 Q002 R005
G76 X0.550 Z-0.9 P21 Q001 F.0590
G00X0.460
Z6.0
M30

Next question is their a possibility that a parameter is wrong or off for this not to work?

thanks,
Zw

[dcoupar]

T0202
S100M3
G00X0.514
Z.1
G76 P030160 Q20 R0 (Q20 = 0.0020 MIN D.O.C.)
G76 X0.550 Z-0.9 P210 Q60 F.0590 (P210 = 0.0210 HEIGHT / Q60 = 0.006 DEPTH OF 1ST PASS)
G00X0.460
Z6.0
M30

[sinha_nsit]

Originally Posted by ZWM51 G76 P030160 Q002 R005 G76 X0.550 Z-0.9 P21 Q001 F.0590

R should be in inches. So, you specified 5 inches finishing allowance!
If you desire, you can specify some value for R in the program given by Dcoupar.

[sinha_nsit]

Incidently, the depth of metric threads is calculated by 0.61344 x pitch.
Bore dia = Outer dia - pitch
Root dia = Bore dia + 2*depth of thread

So, check your values, if you are making metric threads.

[dcoupar]

I believe the actual height should be .0341

[sinha_nsit]

For ISO metric threads, the formula given in textbooks has been copied by me. The thread calculator software posted here does not appear to be using these formulae.
I am confused!
Are we talking about metric threads?
At least, difference of major and minor diameters should be twice of height.
Are practical values different from theoretical values?

[ZWM51]

THANKS FOR THE HELP THE FIRST TELL U THAT THE SMALLEST CUT IT WILL TAKE IS .002
AND THE SECOND Q TELLS U THE DEPTH OF THE FIRST ROUGHING PASS WITCH WAS .006
SO SINCE IT IS .006 OFF BOTH SIDES IT SHOWS .0012 ON THE POSITION PAGE THEN IT TAKES .004 A PASS AFTER THAT UNTILL IT REACHES THE MAJOR DIAMETER WHAT CONTROLS HOW MUCH IT TAKES EACH PASS DOES THAT CHANGE WHEN U CHANGE THE THREAD HIEGHT