Programming thread mill cycle

[squirrelledm]

Can any one tell me how to program a thread mill cycle by hand. I have all the cam system to do this but I would love to know how to do it by hand. Use 3/8"-16 internal thread for an example.

[JPMach]

If you buy a greenfield thread mill you can call up their tech guys and give them all the specs and they will fax you a program thet they gauruntee. Of course now that kennametal bought them out, they are hard to find. I use to be able to find them on kennametals site but now it looks like they have hidden that extra deep in there.

other wise for a right hand thread it is just start at the bottom and do a cicular comp on move on to the wall of the hole and then a circular interp to the same posistion but up one pitch of the thread in Z (or if your machine can't handle that you may have to break this arc into quadrants) and then do a circular comp off move. Greenfield reccomend at least two passes three if you can.

Of couse if using a single point tool then you will need to circular interp with the pitch in Z however many times it takes to get out of the hole.

JP

[psychomill]

Here's one way with perpendicular entry. This is assuming a 1/4" cutter:

T1M6( THREADMILL )
G54.1P1X0.Y0.S6000M3
G43H1Z.1M8
G1Z-.5F50.
G41D1X.0625F10.
G3Z-.4375I-.0625
G1G40X0.
G0Z.1

Or with an arc entry:

T1M6
G54.1P1X0.Y0.S6000M3
G43H1Z.1M8
G1Z-.5F50.
G41D1Y-.0625F10.
G3X.0625Y0.Z-.4844J.0625
Z-.4219I-.0625
X0.Y.0625Z-.4063I-.0625
G1G40Y0.
G0Z.1

If you have a CAM system, just anylize what the CAM system is doing when it threadmills. Think of threadmilling as just a simple "endmill" contour of a circle with the added Z move for the pitch of the thread.

Here's a link to Carboloy . Look on the bottom right and you can download a threadmilling wizard for free. And here's a brief summary of the principles in threadmilling from Scientific Cutting Tools.

Vardex also has downloadable info on this.

[justCNCit]

the tricky part with threadmilling is knowing how the machine handles the G02 and G03's.

Thread mill programming involves using the same start and end point when doing arcs, assuming the control interprets such as a complete circle. Otherwise it may require more elaborate programming.

The second trickiest thing is the start and end of thread mill - you will be starting at 180 degrees from start one half pitch up and begin the full thread at zero degrees and one full pitch. End the opposite way.