[FFWD]

Hey guys. I need help with this. Not used to using taps in a CNC machine...only by hand with my trusty can of Tapmagic through the years.

Recommendations for the best tap to use in this application.

Aluminum
Blind hole
3/16-24 size
tapping depth .800
stopping tap .600 from bottom hole (total hole depth 1.4)

I'm using a VMC for the job. The hole is pre-drilled with a .328 drill bit.

The machine does not have rigid tapping. I use a compression/retention holder for the tap and spin it at 500 on a G84 cycle.

Any advice on this? Taper, plug, bottoming, spiral, straight, HSS, Cobalt, jeez I really don't know. lol

Want a decent tap for the job. Production environment.

Thanks a bunch!

[Geof]

Spiral flute machine tap, Emuge or something like that.

Good rich coolant mix, 10 to 15%.

Run at 1000 rpm or so, drilling .8 and tapping .6 you have plenty of clearance to afford a little overrun.

[FFWD]

BTW...I didn't mean to type "3/16"...it is "3/8".

Long day.

[FFWD]

Spiral flute machine tap, Emuge or something like that.

Good rich coolant mix, 10 to 15%.

Run at 1000 rpm or so, drilling .8 and tapping .6 you have plenty of clearance to afford a little overrun.

Yessir!

Does it matter if it's a taper, plug, or bottoming tap in this case? I'm thinking bottoming.

[fizzissist]

Spiral flute machine tap, Emuge or something like that.

Good rich coolant mix, 10 to 15%.

Run at 1000 rpm or so, drilling .8 and tapping .6 you have plenty of clearance to afford a little overrun.

I just got through a job running a 5/16-18 3fl spiral bottoming, uncoated, in alum, drilled .9dp, tapped .75 deep, one pass, at 1000rpm with rigid. Lots of 10% flood coolant.

Piece of cake, and the tap still looks new! This just happened to be an OSG, but I love Emuge equally.

...btw, you really do want a spiral that brings the chips up out of the hole rather than push them down and pack 'em into the bottom.

[FFWD]

I just got through a job running a 5/16-18 3fl spiral bottoming, uncoated, in alum, drilled .9dp, tapped .75 deep, one pass, at 1000rpm with rigid. Lots of 10% flood coolant.

Piece of cake, and the tap still looks new! This just happened to be an OSG, but I love Emuge equally.

...btw, you really do want a spiral that brings the chips up out of the hole rather than push them down and pack 'em into the bottom.

Nice! I'm looking forward to using a spiral flute tap. Never have. The machine has always seen the plain Jane straight flute bottoming taps for this op.

[Bob La Londe]

Definitely Spiral Flute. You have to draw the chips out of the hole. Does your tap holder have a maximum speed limit? I use a tapping head and tap most holes manually myself, and I think mine has a max recommended machine speed of 750 RPM.

[FFWD]

Definitely Spiral Flute. You have to draw the chips out of the hole. Does your tap holder have a maximum speed limit? I use a tapping head and tap most holes manually myself, and I think mine has a max recommended machine speed of 750 RPM.

I have no clue on its max RPM as it came with the machine. I do know it's a big ol' honker of a holder. It could double practically as a beater stick.

I'm happy at the speed it currently uses. Drilling and tapping is just a small portion of what the overall op I'm doing.

[txcncman]

For aluminum, form taps are highly recommended.

[fizzissist]

For aluminum, form taps are highly recommended.

Good point.... with one serious caveat....

If you go to a form tap, you need to make sure the hole dia is held well within the tolerance (NOTE that the hole is bigger than a normal tap drill size), and you're using a good coolant concentration to keep the tap lubed adequately. (ok, two)
I'll usually shut the coolant off for that op, blow the holes out and dab a touch of Moly D at the top of the holes. I've never broken a tap and the threads have always been excellent.

Thread formers give an excellent finish and stronger threads, while generally requiring less torque and making no chips.

[Bob La Londe]

Good point.... with one serious caveat....

If you go to a form tap, you need to make sure the hole dia is held well within the tolerance (NOTE that the hole is bigger than a normal tap drill size), and you're using a good coolant concentration to keep the tap lubed adequately. (ok, two)
I'll usually shut the coolant off for that op, blow the holes out and dab a touch of Moly D at the top of the holes. I've never broken a tap and the threads have always been excellent.

Thread formers give an excellent finish and stronger threads, while generally requiring less torque and making no chips.

I have had good luck with form taps in aluminum, but again I use a tapping head with a slip clutch, so if I get a bind I just let go of the handle and it reverse out. I would add that I tend to use a drill a few thousandths smaller that the one reccomended in the form tap chart I printed out and added to my "Pink Book." It just "feels" better usually.

The Pink Book is a three ring binder I keep in the shop. When I find something I think I might need to refer back to regularly I print it out and add it to the binder. Drill size chart, tap drill chart, drill speed chart, metal thickness gage to thousandths size, melting points, hardness table, etc etc etc... I use it all the time when I am working in the shop.

[JimBoyce]

Since you do not have rigid tapping, check to see how much dwell the machine has at the bottom before the spindle reverses. This maybe a parameter setting, and if excessive can cause the tap to go deeper than anticipated (snap).

[fizzissist]

Since you do not have rigid tapping, check to see how much dwell the machine has at the bottom before the spindle reverses. This maybe a parameter setting, and if excessive can cause the tap to go deeper than anticipated (snap).

Ah... So THAT'S what that noise was...

For a tapping head (which I don't use in the mills anymore since rigid) I would program the feed ever so slightly less than the lead. This seems to allow the tap to pick up an existing thread if I wanted to go in for multiple depth passes. With a tapping head I'd also drill as deep as I could get away with because of the unknown Z where the head would release and begin to reverse.

These techniques have worked well for me over the years... but as always, I'm open to suggestions and new ideas!!

[FFWD]

Thanks a bunch for all you guys' input on this! It's helped me a lot.

To answer the question about dwell, I have that parameter setting in my software. I have it set pretty well and have it down to about .010 to where the threads needs to stop. It was a few times of sneaking up on it to figure out, but I'm comfortable with it now.

I've now ordered a spiral flute from Emuge...I'll see how it goes. Expensive little sucker.

I also think I'll take the advice of an earlier poster and stop the coolant at that tapping cycle and add something like Tapmagic to the holes before I hit the start button. I never run my coolant that rich (that apparently taps like) so it might be better for me to do it that way from here on out.

[Bob La Londe]

TapMagic all metals is pretty awesome stuff. I use it for just about all my manual processes now, and I used it for some fairly long 3D CNC milling jobs in aluminum where I was just clearing chips and cooling the metal with air. I was amazed with the results. Few drops rubbed all over the surface made a huge difference over dry cutting. They also have a formulation for aluminum specifically that is supposed to be even better, but I have not tried it.

You do want to make sure you get All Metals or Aluminum forumaltions, as there is one Tap Magic formulation that makes a grey mess when used on aluminum.

[Edge Finder]

I thank to form tap is your best idea a little Mole D you cant go wrong.

[BAMCNC.COM]

I'd check eBay for "TAP Lots" too. Last year I got 172 spiral flute taps for 126$, just one of those taps is worth 120$....

[MetalZilla]

I use Roll taps in aluminum whenever possible. eliminates the chip problem. also you may want to check out these tapping formulas: Tapping and Threading Formulas