Hi,
Has anyone successfully used a Tapmatic on a standard 3-axis CNC mill i.e. one without spindle position control?
TIA, Alan
Printable View
Hi,
Has anyone successfully used a Tapmatic on a standard 3-axis CNC mill i.e. one without spindle position control?
TIA, Alan
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.
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...
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=CkTo...&index=49&t=0s
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.
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?
>>> 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.Quote:
Originally Posted by alanambrose
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.....
Attachment 28304
Oh good. The photo has rotated during upload.
Attachment 28305
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_ins...e_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.
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.