Okuma G71 Lap help

[NathanJWilliams]

So I have looked many places for this and can’t find the answer. I’m working on a Okuma LB25 with a OSP500 control. I’m trying to single point a M55x2.0 at an inch long and I have the code written out after a while of trying to figure it out (only CNC machinist at my job)
G0 x2.1720 Z.5
M8
G71 X2.0786 Z-1.03 B00 D.001 U0 H.0834 F.0787 M33 M74
G0 X3.5
M9
Etc.
Every time the inserts get about .03 into the part it begins to just take off way too much and even though there is still .06 or so left to cut in the program the threads are already oversized. This is my first time making a post and idk if it’ll work but thanks in advance for any help!

 

[Booze Daily]

For starters, I would increase your clearance diameter. You are only .008 above the OD.
B is the infeed angle. You are plunging straight down the middle of the thread. I would change it to B60.
D is the depth of cut based on M74. It's going to cut .001 per pass until it reaches (H-U). So your going to make about 84 passes.
M33 is zig zag infeed. One pass along right face of thread, next pass along left face of thread. It only works if you use a B value that's not zero.

There is also an M code that specifies how to pull out at the end of the thread. I don't see it in your code and don't know what the default is.
M22 will pull straight out, used when threading into a relief. M23 will chamfer out of the part, used when there is no thread relief.

You said your threads are oversize when you still have .060 to go? They should be. By about .060.
Or did you mean undersize? Could be the thread isn't happy being cut right down the middle.
You don't mention the material or how far away from the chuck your thread is, but at .0005 depth of cut it's possible the insert just rubs and rubs and then takes a shit ton of material all at once.

 

[DouglasJRizzo]

Have your clearance diameter at least .15" over the major (I use .25") and start a minimum of .25" in front. I also use M22 straight pull out.