Tension/compression heads for CNC tapping

[DavidR8]

Hey folks, as I get closer to making chips with my CNC mill conversion I got thinking about tapping. The Masso controller I'm using doesn't support rigid tapping so thread milling is my go-to. But then I saw a tension/compression tapping head and thought that could work.
Had anyone used one for tapping on a CNC mill?

 

[mmcmdl]

Hey Dave . I have a few that I used on CNC lathes/mills . I can get some pics if you want .

 

[BGHansen]

Following your thread. I have a T/C head for my Tormach 1100S3 but have never used it. I don't know the inner workings, but mine "behaves" like the driven shaft and tapping chuck are keyed to each other and are spread by a compression spring. I attached Tormach's guide for using the head. Hope this helps a little though someone with actual experience will be the best teacher.

 

[mmcmdl]

That's a nice set ! The programming brought back good memories also . I would always program the feed rate as the thread pitch minus .001 per rev though . Seems as though they tie the feedrate to the rpm .

 

[mmcmdl]

Royal Products . I had a nice pair of Hardinges but sold them on the bay a while back .

 

[dbb-the-bruce]

I have this one from Tormach worked great the few times I've used it (new machine, so don't have a lot of experience with it)

There is a little bit of a trick to it - you have to make sure that the tapping cycle G-code doesn't have any dwell programmed. This can depend on what you are using for CAM and the post.

The gist was that with Fusion 360, if you leave dwell out of the dialog box it wouldn't add a dwell value to the tapping / drill cycle and there was some default. However if you specify a very small dwell .0001 seconds the value gets used and truncated to 3 digits and it spits out a dwell of 0.

The head has enough allowance in tension/compression to accommodate a spindle speed that doesn't exactly match the tap threads in additions to being able to handle the spindle reversing.

I believe there is a NYC CNC video about it.

 

[Chipper5783]

I have the “Synchronizer” from Shars in ER16. I’ve done about 1000+ holes #8 to 5/16” - very happy with the results (except for the time I didn’t drill a hole first, that did not end well - there is a story there that I don’t feel like sharing).

Interested in adjusting the advance rate to slightly below the thread pitch lead? What does it gain - a little better surface finish, maybe some forgiveness on the bottom hole reversal (keep everything in tension)?

 

[BGHansen]

I have the “Synchronizer” from Shars in ER16. I’ve done about 1000+ holes #8 to 5/16” - very happy with the results (except for the time I didn’t drill a hole first, that did not end well - there is a story there that I don’t feel like sharing).

Interested in adjusting the advance rate to slightly below the thread pitch lead? What does it gain - a little better surface finish, maybe some forgiveness on the bottom hole reversal (keep everything in tension)?

The problem with my Tormach is that the spindle RPMs on the controller display is not 100% accurate; it doesn't have an encoder that measures actual speed. I've never adjusted it, there is a pot on the VFD of my Tormach where the RPMs can be adjusted. It can be done with a Hall-effect tach on the spindle; adjust the VFD so the Hall-effect tach matches the controller's indicated RPMs.

I'm thinking (scary) that the Z-axis feed should be slightly faster than the spindle speed so the tapping head compresses slightly as the tap advances. If the Z-axis feed is too slow, the spindle would be turning the tap faster than the Z-axis feed; the tap would advance at a rate faster than the head possibly pulling it out the the chuck or snapping the tap (?). The Tormach head has about 1/4" of travel in compression; going too fast in Z "should" result in the head compressing as it's designed to do.

This is a snippet of Tormach's instructions:



Using their example, a 1/4-20 tap running at 500 RPM would need a feed rate of 25 IPM (500 / 20); feed rate = spindle RPM / tpi. The concern is that my machine may say the spindle is at 500 RPMs, but it may be 450 or 550 since there's no encoder/tach built into the machine. If my spindle was turning at 550 RPM, the feed rate should be 27.5 IPM (550 / 20). I'm thinking (again, scary) that it'd be prudent to go slightly higher on the Z-axis feed than the calculation to compensate for inaccuracy in the spindle RPM. If I were going to use the head, I'd do the procedure in the Tormach manual for adjusting the VFD pot to get as close as possible to the spindle speed at which I'd be running the tapping head.

If I'm correct in my thinking (all theory, no experience), a slightly high Z-axis feed rate would mean that the head is compressed during tapping. The Tormach head has about 1/4" of compressive travel, so there's a little wiggle room depending on the depth of the tapped hole.

Anyway, don't take anything I said as the gospel; it's my understanding of how it works with no experience.

 

[mmcmdl]

Floating holders . The heads are bottomed out when starting the tapped holes . Feed per rev being just under the pitch allows the head to pull forward at the pitch. Instant reverse . Head reverses and still pulls head out until threads are cleared . Head snaps back to closed position . When reversing ,you can program a lead over the pitch as well as the head would be extending . I never did and never had issues .

 

[mmcmdl]

I have the “Synchronizer” from Shars in ER16. I’ve done about 1000+ holes #8 to 5/16” - very happy with the results (except for the time I didn’t drill a hole first, that did not end well - there is a story there that I don’t feel like sharing).

Well , why did you mention this holeless tapped hole ? Come on , spill the beans !!!! Believe me , I could tell some stories also .