Tapmatic on CNC mill?

[alanambrose]

Hi,

Has anyone successfully used a Tapmatic on a standard 3-axis CNC mill i.e. one without spindle position control?

TIA, Alan

[Muzzer]

No but it's something I'd love to bottom out at some point soon. I can't sensibly rigid tap on my Acorn machine due to the need for a directly connected spindle encoder which isn't really practical on a turret mill.

I have a Tapmatic clone, so that would be a pragmatic compromise. If you plan to have a go, I'd be interested to see how you get one and might be provoked into joining in for the ride.

[alanambrose]

Well I can't imagine it's that hard as those things are meant to be used with a normal meat-driven pillar drill. It would be nice to find someone who had actually done it though...

[Muzzer]

Main ballache will be restraining the reaction arm. There's nothing obvious to anchor it to on my machine, as the quill disappears back into the head where it needs to be to find its home switch.

I may need to figure this out shortly, as I will soon have a shit load of M4 and M5 threads to do and a cordless drill doesn't seem to be the way to go. I need to get my act together...

Some bald guy on the Tormach channel has done an intro video to it. As he points out, the feedrate is the rpm times the pitch and the retract rate needs to be double the feedrate.

https://www.youtube.com/watch?v=CkTo46ov7FA&list=PLqsHVR4MZg_gRBCj47zpCLkxHKXRGsGrc&index=49&t=0s

[Muzzer]

You can see the g code around 7:00 in the vid. It's fairly simple I suppose. Being a Mercan, the units are inches:

S1000 (1000rpm in his example - he's not paying for any breakages)
(goto x,y hole position)
G1 Z-0.25 F12.5 (feed down to 1/4" below the surface - it started 1/4" above the surface from the previous operation)
G1 Z0.25 F25 (retract back to 1/4" above the surface)
(goto next x,y hole position)

etc

The tap he is using is a tiny gnat's cock thing with 80TPI ie 12.5 thou pitch, so at 1000rpm, the feed rate needs to be 12.5 (inches per minute). And the retract feedrate is twice that ie 25 (inches per minute).

I suppose the way to do it may be to write a little macro like the above and call it up using the manual NC option within Fusion CAM for each hole position? I don't want to manually type in the coords but I can't see how to make it happen from Fusion.

[Muzzer]

Doesn't look too difficult actually, famous last words. You tell Fusion you have a drill, not a tap. That way you can control the feedrate by playing in the tool manager to make a new "drill" tool.

For an M4 coarse you need a 0.7mm pitch. That's the "feed per rev" in Fusion terms and it is calculated from the spindle speed and the "plunge feedrate". I entered an expression of "0.7*tool_spindleSpeed" for the plunge feedrate but you could do that in your head. Obviously if you bottle it and decide to reduce the spindle speed, you'd be glad you used the expression rather than a hard coded value

So with 300rpm and 210mm/min, you get 0.7mm per rev. Then type in double the expression ie "1.4*tool_spindleSpeed" for the retract feedrate.

No buggering about with macros after all if I'm right here.

The other clever bit would be to set the "bottom height" to be somewhat higher than the bottom of the hole. I'm afraid that human element is where the wheels might come off.

EDIT - my Tapmatic clone requires ~3.5mm of travel before it disengages and goes into reverse, so the "bottom height" needs to be at least 1/3 of 3.5mm (plus a margin) from the bottom of a blind hole. It also means there is a min hole depth of perhaps 2-3mm for blind holes. How low can you go?

[alanambrose]

>>> Main ballache will be restraining the reaction arm.

I planned on using a tall stud from a clamping kit mounted on the bed? Maybe with a bit of tube over it for lower sticktivity.

Alan

[Muzzer]

>>> Main ballache will be restraining the reaction arm.

I planned on using a tall stud from a clamping kit mounted on the bed? Maybe with a bit of tube over it for lower sticktivity.

Alan

I was up Dawn's crack this morning before the Domestic Manager got up and as a result managed to get some workshop time in.

In fact I find there's enough of the quill nose poking out in the parked / homed position to get a pinch collar on there. I bought a spindle speeder from JohnS a few years back that fitted his Beaver mill. I haven't used it yet, as it's imperial (NMTB40) rather than the metric of my power drawbar (ISO40). However, being a speeder it also has a reaction arm and came with a pinch collar thing for his machine. Turns out his quill was a couple of mm smaller than my Shizuoka quill, so I was able to bore it out on the lathe and Bob's your auntie - I have a solution. John must be smiling on us from his workshop up there.

I bodged a short length of steel strip into a reaction arm and I screwed a short pillar into the collar to pick it up. So I can remove the pillar when not in use and the tapping head is otherwise self contained. The pillar is made of loominum as it was ready to go but I may change it for steel at a later date if this works out.

Scarily, I have now got a tapping head ready for action and have come to believe that the CAM might be reasonably straightforward. That requires less talking and more machining. I'll think on that as I waste the rest of the day failing to be a plasterer and perhaps give it a go this evening on a piece of scrap.....

28304

Oh good. The photo has rotated during upload.
28305

[m_c]

I have looked into this previously, but never actually got around to trying it, as I've yet to find a real need for it.

IIRC, all you have to do is program for a thread, dwell for a few revolutions at the bottom, then rapid back out. I can't remember where I found the information (possibly PM forum..), and you need to do a little bit experimentation to get the timings right, as the tap won't always bite at the same point, so you have to allow for a thread or two variation.

Actually, tapmatic have suggested code in their CNC tapping head manual - http://tapmatic.com/product_line_instructions_rct50_reduced_cycle_time _tapping.ydev
The only thing you'll need to allow for if using a non-cnc head, is the standard heads normally reverse out faster, whereas as the CNC heads reverse out at the same speed they go in.

[Muzzer]

Probably not a great idea to "program for a thread", as that generally involves reversing the spindle. Threading generally assumes some knowledge of the spindle position which we don't have here.

In this case we use the "feed per rev" in Fusion CAM to get the correct pitch - and we know when to stop feeding based on the height / z position. It's only really possible to use this method because the spindle speed is known and constant, unlike a rigid tapping move. Once we start to withdraw the tapping head, it takes care of the reversing. That's the benefit of the Tapmatic type head.

If you run your pork pie over the thread above you will see how we have considered how to get the feedrate right for the required thread pitch and also how to cater for the (twice) faster reverse.

I have tension compression tapping heads too but without a spindle positioning system (aka encoder), I reckon trying to control the depth of threading via a VFD would be fraught and expensive.

[m_c]

I'll admit programming for a thread wasn't what I should have written, but


If you run your pork pie

You are a Prick.

[Muzzer]

Bugger. Well that may have been a fantastic waste of time, for my machine at least. When I run the Centroid post processor, I'm getting the correct feedrate into the hole but the retract feedrate is defined within the G81 canned drilling cycle - and worse than that, when I dig into the manual, it's a rapid retract (G0). The Fusion dialogues allow you to set the retract feedrate but the Centroid post processor ignores that and lets the canned cycle handle things.

Presumably, short of rewriting vast chunks of the post processor, I'm stuffed. I could use the boring cycle instead, which retracts at the feedrate but that's not a whole lot better unless you have one of the special (ie rare) tapping heads with the same reverse speed as forward speed.

There's a certain amount of tension movement allowed on the Tapmatic style heads but It's not clear what I could sensibly use there.

The jury is out. Not sure if this has been a waste of time or not until I explore my options....

[Muzzer]

I'll admit programming for a thread wasn't what I should have written, but


You are a Prick.

Bloody hell, that's a bit harsh. But it has been said on occasion..

[Lee Roberts]

Bloody hell, that's a bit harsh. But it has been said on occasion..

m_c, got your email...

What exactly offended you by Muzzer's pork pie reference ?

[m_c]

m_c, got your email...

What exactly offended you by Muzzer's pork pie reference ?

Obviously my interpretation is totally different from yours, and what I said in the email still stands.
Regardless, I'm out of this discussion.

[Lee Roberts]

Hi,

OK, well i interpreted "pork pie" to mean "eye" and that Muzzer came to the conclusion you hadn't read the whole thread as i couldn't see a link to another.

If the above is true then calling him a prick is a bit OTT in my opinion but as per your email i think you already know that.

Unless you've got further issue Muzzer and m_c declaring himself as moved on, I guess we can all move on with more positive things :eagerness:

[andy_con]

This is my Denford triac with a 20 year old tapmatic tapping head.

Amazing bit of kit

https://youtu.be/jR26gs1tvtM

[Muzzer]

I made some useful progress on this. Although Fusion appears to allow different values to be specified, the post simply generates a G84 tapping macro command, which doesn't pass the retract rate. The alternative, closely related tapping / boring canned cycles all use either the rapid retract or the same as the infeed.

The tapmatic would work but the head has to soak up a fair bit of axial movement as the spindle withdraws at the wrong retract rate. May be fine in most cases but for longer holes and coarser pitches it could get a bit iffy. Other issue for my machine is that the reaction arm collar mounts on the threaded nose of my quill that holds the main bearing in place. During the retract, the reaction arm tries to unscrew it, which wouldn't be ideal if it succeeded.

Given these and the fact that I also had a tension compression head and a fair selection of collets, at this point I changed my focus from the tapmatic method. Although I got it working I've now put it back in the cupboard and may bring it out later for use with the Bridgeport.

The tension compression approach is simple enough to implement, the main difference to the tapmatic being that you have to stop the spindle and reverse it, ideally in synch with the infeed and retract moves. The std G84 works fine as long as you don't try to run it too fast. The main difference between this and rigid tapping is that you don't need a spindle encoder.

My tension compression head seems to have around 8-10mm axial movement either side of the unloaded position. But if you are running slow accel and decl times in the VFD, there can be a fair amount of overshoot, so that the tool is still going forward while the spindle has started retracting. I have a braking resistor in my Yaskawa VFD but even so, if I set the decl time to under 1 second, I can't run much more than 400-500rpm without overvolting the VFD. You don't want that to happen with the tap at the bottom of the hole.

Given the need to sharpen up the start and stop times for the spindle (increasing the risk of overvoltage), it's a good idea to tie the VFD error signal into the controller, so that the machine will stop if you cause an overvoltage and the spindle stops. It took a bit of fiddling to optimise the accel / decel rates against the max speed I could run. If you are going to be using a larger tap, there will be less chance of the VFD overvolting as the spindle will be running slower and there will be more torque required to drive the tap. So I did my tests on a thin aluminium section with a small (M4) tap.

Not the most exciting video you will ever see but here's what I got:

https://www.youtube.com/watch?v=6rsnMqoHHNM

I'll be doing some more challenging tapping into aluminium plate shortly and hopefully they will go OK now...

[JAZZCNC]

Hi,

OK, well i interpreted "pork pie" to mean "eye" and that Muzzer came to the conclusion you hadn't read the whole thread as i couldn't see a link to another.

If the above is true then calling him a prick is a bit OTT in my opinion but as per your email i think you already know that.

Unless you've got further issue Muzzer and m_c declaring himself as moved on, I guess we can all move on with more positive things :eagerness:

Ah ah it's nice for a change for it not to be ME getting a slap on the wrist for my creative choice of words. . .:lock down fever I reckon ::hysterical::hysterical::hysterical:

[Muzzer]

Slightly more convincing demo with M8 x 1.25 machine tap. At least I have a slip clutch collet for this one:


https://www.youtube.com/watch?v=XmPVVvQptcU