[zerodegreec]

The BF20 CNC is the bees knees, but without a servo like Hoss has or a lathe to make the stepper motor tapping setup he has for the X2 I would like to find some options. Seen the compression/Tension tapping heads on Shars and they look like the way to go. I do not have any ER collets and the ER20 seems to be the range that I would use the most.
Attachment 181650

Thoughts? should I look at a auto reversing?


shars.com
shars.com

[SCzEngrgGroup]

Look into thread-milling. No special machine capabilities required, just a thread-milling cutter (which, in a pinch, can be made from a hand tap), and normal CNC operations. It will even thread to nearly the bottom of blind holes, which you can't do with a tap. And, you can do a variety of different thread sizes, and both inside and outside threads, and left-hand and right-hand threads, with a single tool.

External Thread Milling with a Tormach PCNC 1100 - YouTube

Regards,
Ray L.

[zerodegreec]

I actually have a 60deg v-slot cutter and I will have to give this a shot for external, unfortunately it is a 3/8 diam tool and I am needing to do bout 50+ M10 1.5 holes. Will look for info on how to make one out of a tap like you suggested.

Edit: seems all I have to do is sacrifice a Tap and grind off all the teeth except one.... Tomorrow is going to be a good day for testing

[hoss2006]

yeah, you must have missed this video, a ground tap makes a good threadmill.
Be sure to cut the relief on the tooth.
Hoss

[hoss2006]

And you can get creative with it.
Hoss

[hoss2006]

I also think you should really consider getting a lathe, even a little 7x can make lots of parts you may need.
Lots of links here under Lathes.
G0602
Good luck.
Hoss

[hoss2006]

One more option then I'll quit bothering you.
A reversible tapping head is a great thing to have, it can mount in a drill press or the mill with an adapter for quick easy tapping.
No need to reverse the spindle, the head does it when you lift back up.
This size is good for up to M12.
Reversible Tapping Heads (WT)
Check ebay for better deals.
Hoss

[zerodegreec]

Great stuff Hoss, thanks. How did you change the configuration in Mach or your CAM program to do the horizontal threading? Trying to get my head around that one.

[hoss2006]

I used G19 (YZ plane) instead of the normal G17 (XY plane).
Here's the program.

G0 G49 G40 G19 G80 G50 G90
(TOOL DIA. 0.5)
G20 (Inch)

G64
G00 X-.500
(Right hand OD Conv)

Z1.036 Y-0.2875
G00 X-0.5
G01 Z0.7485 F10
G02 Z0.435 Y0 R0.2875
G03 Z-0.435 Y0 R0.435 X-0.4355
G03 Z0.435 Y0 R0.435 X-0.4231
G03 Z-0.435 Y0 R0.435 X-0.3846
G03 Z0.435 Y0 R0.435 X-0.3462
G03 Z-0.435 Y0 R0.435 X-0.3077
G03 Z0.435 Y0 R0.435 X-0.2692
G03 Z-0.435 Y0 R0.435 X-0.2308
G03 Z0.435 Y0 R0.435 X-0.1923
G03 Z-0.435 Y0 R0.435 X-0.1538
G03 Z0.435 Y0 R0.435 X-0.1154
G03 Z-0.435 Y0 R0.435 X-0.0769
G03 Z0.435 Y0 R0.435 X-0.0385
G03 Z-0.435 Y0 R0.435 X0
G03 Z0.435 Y0 R0.435 X0.0385
G03 Z-0.435 Y0 R0.435 X0.0769
G02 Z-0.7485 Y-0.2875 R0.2875
G01 G40 Z-.900
G00 X-.500

M30
M02

Hoss

[zerodegreec]

have to ponder that aspect once I get my head around more of the functions of the CNC.

I successfully made some thread milling holes, turned out well -although I made a mess of the tool and the threads need to be chased-
Can a thread milling be setup as a canned cycle for multiple holes? Rather than manually moving the via MDI and running the cycle for each hole?

[hoss2006]

Sure, Bob has a good explanation of using subroutines.
G-Code Tutorial: Subprogram and Macro Calls
The tapping code would be your subroutine that you would write once and call it however many times you need.
Hoss

[zerodegreec]

Edit:
Figured out how to do it with HSMEXPRESS. Setup a bore operation. Made a tool with the diameter of the cutter. Made the holes in the model the major diameter of the hole I am threading. I set the pitch and center option of the bore for when it retracts. And off she goes

Took me about 3hrs to figure all of this out and it would have taken a third of the time to do it "manually" using the wizard. But this is how we learn and get more efficent. Thanks for the tips Hoss and HimyKabibble
:cheers:

[zerodegreec]

Duplicate Post

[zerodegreec]

Anyone have some good sources for single point tooling? I found Micro 100 and the prices are reasonable. What are you doing and what sizes are you finding the most useful? I do allot of metric from 2mm and the largest is 10mm. Imperial is from #2 up to 3/8 but I have no need to thread mill anything smaller than #6 as I do this with the mill by hand (hand feed the quil and turn the spindle by hand to feel the threads cutting)

Are you just making your own from old taps as you need them?