So I assume doing this will still allow the machine to line up with the original thread? Also for normal 60 threads, do you use 60 for the thread angle or do you use 30 like you would on a manual lathe(actually I usually use 29 1/2 on a manual). Or do you have program it at 0 degrees if you want to run a finish later? Sorry for the questions but I have to have this this all figured out before I pop a 12' shaft in this lathe that needs threads. Something small if I messed it up wouldn't be a big deal, but scrapping a 12" dia. x 12' long shaft is quite another.
Hello cuttergrinder,
Its as Seymour suggests with regards to taking an additional pass (passes) at full depth, the Q value is specified with the P value of the 2nd G76 Block.
The angle specified if you want only the Leading Edge of the insert to cut is the Included Angle of the Thread Form (the included angle of the Threading Insert), not the Angle/2. Specifying any angle less than the Included Angle of the Thread Form will have the Insert cutting on both the Leading and Trailing Edge, but more on the Leading Edge until a Zero value is specified. At Zero, the same amount is cut by the Leading and Trailing edge of the insert.
In addition to ensuring that the same Z Start Point and Spindle Revs be used when repeating a G76 Threading Cycle, when programming to take an additional pass at full depth with another G76 Cycle, its important that the same Angle and Thread Height that was specified in the "Threading from Scratch" G76 Cycle be specified in the full depth repeat G76 cycle. The control uses the following algorithm to calculate a forward shift of the tool at the Start to accommodate a Thread Form Angle specified in the G76 Block
ZShift = TAN(A/2) x (d x sqr
)
Where:
A = Include Thread Angle specified
d = First Pass DOC (Q Value of 2nd G76 Block)
n = nth number of Threading Pass (1st, 2nd, 3rd and so on)
It progresses this way until d x sqr
- d x sqr(n-1) is less than the Minimum DOC that is specified (set). Ultimately, the DOC will equal the Thread Height, therefore, if the same Thread Form Angle and Thread Height is used in both G76 Cycles, then the Threading Tool will track the same path.
Regards,
Bill