Thread Milling

Flycut · November 02, 2021, 03:43 PM

What do I need to do to get more than 1 revolution from my thread milling operation?
MC2020
Like overlap so I can cut slightly past my start point.
TIA

gcode · November 02, 2021, 04:45 PM

Lie about the number of teeth on the cutter

Jeff · November 03, 2021, 04:16 AM

Yep. If you tell it there is 1 tooth, the cutter will follow the entire thread.

gcode · November 03, 2021, 04:52 AM

It would be nice if they had an overlap setting when more than one depth pass is required
Sometimes you have to lie about Top of Stock as well to prevent oversizing the top portion of the thread

Flycut · November 03, 2021, 05:06 AM

Lying about the teeth only cuases the tool to make one rev then move up and repeat at a different depth.
Still no overlap. Using one tooth gives me 8 revs but I only need1.25
I'm doing 12 holes per part. The 7 extra revs turn my 4 min cycle into 45
I'll try messing with the top of stock.
That might be the ticket.
(1 tooth + top of stock = win)

neurosis · November 03, 2021, 05:15 AM

If you follow what Jeff said and change the number of teeth to 1, it will follow the entire thread. Not the perfect solution but probably the only one.

It really does need an overlap setting.

neurosis · November 03, 2021, 05:16 AM

responded before you changed your post.

gcode · November 03, 2021, 06:00 AM

how many teeth does your thread mill have?
how deep are the threads and what is the pitch?

Flycut · November 03, 2021, 06:11 AM

hole 8-32 by 0.200 deep
Tool mtec 0250c02 32un ( 8 teeth )
Ended up programming to 1 tooth 0.200 deep, top of stock -.15
Worked just like I needed
Now I need to find the gauge.