Tapmatic chuck in a CNC mill ?
My older Milltronics does not support rigid tapping. I tried to tap using a floating collet in my collet chuck, but this does not really work with repeatable results. ( accel/ dwell/ reverse )
I have a tapmatic that is good up to 5/8 " tap . Anyone ever try running this as just another tool in the carosel ? . I can put a stop rod in a bolt hole on the head . The reverse ratio is faster on the withdraw , so I can just move the z up a bit faster .
Figure I can just write a sub program/ call that has a z down, z up .
the only problem I can see ,is how to make sure the stop arm does not crash into the rod mounted on the head when it does a tool change . The machine does do a spindle orient at every tool change , but how can I make it do a 1/2 rotation to swing the arm away from the stop ?
How about putting the stop rod on the vise ? then it can just raise up when I change tools .
I see a true CNC tap head is constructed a bit different in the way it registers in the spindle , but never actually saw one up close
Cnc tap heads have a little arm at the top, with a dog on the spindle housing. Since tools get put away in the same orientation as they get loaded, you should be able to figure out a way to keep the stop rod located approximately in the right place. Your stop rod doesn't have to be rigid, it just has to keep the head from spinning. That said, you can put a large ring or socket on the spindle housing and allow for a little slop in the rod. Mount the rod to the tapping head, not the spindle.
we use them in some of our mills we just use a g85 boring cycle with the proper feed etc. and we just use a bolt with a bent rod welded in it that goes into one of the bolt holes on the spindle,works just fine.we have matsuura vmc's and they do spindle orient as well.
I think some are missing your point Bob.
What you are asking is scary.
Think Snow Eh!
Can you make a plate to bolt on top of the tapping head and remove a bolt from the spindle seal housing and replace it with a threaded stud, maybe with a washer and nut to keep the torque even on the seal housing? That way you have the rod in the spindle not sticking out of the tap head. The shop next door did this on a cincenatti (spelling?) and were tapping twice as fast as rigid tapping.
Why not just buy the proper Tapmatic head? It will hold 0.004" on depth and tap probably 5x faster than you can now. So it will pay for itself over time.
If one of these Rube Goldberg set ups breaks the ATC, draw bar, pull stud collet, or worse yet comes apart when it's running you've saved nothing.
At the very least copy the way that Tapmatic does it. They've got thousands of these things out in the field.
The stud in the seal housing IS the way that Tapmatic does it, Thats not quite Rube Goldberging it, that is the way the Tapmatic guys told the shop to do it!
Here's a novel approach, do a manual change, then it's not an issue. If you are tapping a zillion holes in one op, this will be economical. If you're doing 2, do it offline with the drill press and the tapping head. Or find a used tapmatic CNC head. $2k for a tapping head is a good chunk of what that machine is worth.
I use Tapmatic heads on our big Monarch 150 all the time. From #4 to 1/4" taps. Bigger taps I use the control's "air tap" cycle. (basically the spindle goes into a free floating mode and the tap winds itself in, spindle reverses and the tap winds itself out, but I digress.)
If you can, lock the feed and speed calls (our machine uses G63 on, G64 cancel) so you don't pull the thread if your rpm and feedrate overrides aren't exactly 100%.
With our Tapmatics we found it best to program the feed slightly slower than the pitch, if you follow, the tap has a little end float.
We use a G85 feed in/out, and a .500 "R" plane, since the taps need a little extra time (floating) to clear the part before moving to the next hole.
Speeds and Feeds for our most common tap sizes:
4-40 300 RPM, 7.125 IPM
6-32 300 RPM, 8.9 IPM
8-32 300 RPM, 8.9 IPM
10-32 300 RPM, 8.9 IPM
10-24 300 RPM, 11.875 IPM
1/4-20 400 RPM, 19.0 IPM
Hope this is of some help.
A manual tool change is not the answer I am looking for , although that would be the safe move . I don't think my tool changer cares what kind of tool I put in the carousel.
I plan to put 4 pcs each in 2 vises . Drill /cbore/cfr / optional stop to apply oil /tap .
I have 4,000 parts to make in batches of 500 . It may turn out that the drill/cbore cycle time is equal to a manual tap operation . I see the ads for the cnc tapmatics , and it looks like there is a restraining post on the top ring that has a generous taper. so I would guess that an engagement socket with a large tapered female bore , mounted to the spindle ring would allow for any mis alignment . There seems to be a bit of internal resistance in the tap head , so that the engagement post would stay in the same orientation after it leaves the spindle . I tried to download the tapmatic pdf someone posted , but is a bit of a large file .
Anyone have a photo of one in actual operation ?
Thanks FB Bob
Here's a different Tapmatic link; a bit smaller pdf file. They also have some blurry vids on their home page.
Thanks for the link . This will help a lot . My Tapmatic is a manual , and retracts at 1:75 %
I am assuming that a CNC unit is a 1 : 1 in /out . not a big deal to write a program that feeds up at a higher fpm .
I think I will just do it as simple z moves and leave the feed override controls active .
A programming friend offered this trick : mount a feeler , or strip of banding iron to a vise, and position it so the tap engages the edge in the root of the tap . That way I can tap air , and see how it feeds and retracts without breaking things .
I've ran tapmatic heads on a VMC for yrs. But never entertained what your talking about.
I have bought two brand new Tapmatic CNC heads off E-Bay for $300 each. I think they both came with Cat50 tapers yet to boot! (Not just the 1" straight shank.) You can buy them all the time on there for that kinda $. I can't imagine fussin with that drill press unit!
Think Snow Eh!
Just out of curiosity, what model of Milltronics CNC do you have there? I thought most of their vmc's support rigid tapping...? Peace
Nikken auto-depth floating tap holder! No arm involved and super accurate depth control on machines that don't have rigid tap. I just ran a batch of parts with a .600 deep blind hole and tapped to .550 usable thread with a 1/4-20 bottoming form tap. I think I could have easily pushed it to .565 which would have left about .010-.015 between the end of the tap and the bottom of the hole. Uses Bilz collets so easy to change taps too.
Ok, but it seemed he was concerned with accurate depth control. The Nikken will beat the Tapmatic in that. I don't see how the Tapmatic is going to be 4-5 times faster. Additionally, you should have the improved tapping cycle on your Matsuuras that would negate the faster exit speed of the Tapmatic.
Originally Posted by alliancefab
I have 30+ of the nikken holders you are talking about I use them everyday. You can run a faster spindle speed with these because there is no reversing the spindle its just in and out. They are accurate in depth control as well.
Originally Posted by Hot Bob
Not to many good examples in the vid but a few.
As long as the chamfer at the top of your hole and the hole diameter is consistent the depth should stay consistent.