Allied Machine offers an online program generator.
Click here to make your program.

THREADMILL PROGRAMMING HELP SHEET FOR UN INTERNAL THREADS

When programming threadmills the start position in X and Y should be at the center of the drilled hole.  The Z start position will be at the top of the part.  All the programming is done in incremental mode since the absolute hole positions are not known.  All the cutting will be climb milling.

 The last move is to rapid Z out to the top of the part and then go back to "absolute" mode.

 

This is a generic program that may not be suitable for all machines.  Verify that your machine is capable of helical interpolation.  The vast majority of CNC machines manufactured in the last ten years have the helical interpolation capability.  Machines manufactured before that time usually supplied it as an option which can be enabled with a parameter.  The best way to see if your machine is capable is to MDI the part program below into the machine and see if it will make the moves.

It is generally recommended to cut fine threads in one pass and coarse threads in two passes.  If you need to use two passes, just repeat the program below and use a different D word to reduce the depth of the first pass.  If you are cutting a 3/8-16 thread, increase the offset for the first D word by about 35% of the pitch or (.35 * .0625) = .0218

SAMPLE PROGRAM FOR A 3/8-16 x 3/4 DEEP THREAD WITH A .235 DIA THREADMILL

N05

M3 S3521

 

 

 

 

 

 

N10

G01G91

 

 

Z-.7578

 

 

F30.00

N15

G41

X.0350

Y.0350

D(offset#)

 

 

 

N20

G03

X-.0350

Y.0350

Z.0078

i -.0350

j 0

F4.85

N25

G03

X0

Y0

Z.0625

i 0

j -.070

F4.85

N30

G03

X-.0350

Y-.0350

Z.0078

i 0

j -.035

F9.70

N35

G01G40

X.0350

Y-.0350

 

 

 

F30.00

N40

G00

 

 

Z.6797

 

 

 

N45

G90