Has anyone power tapped AL with a tap this large in a mill? Will it work? FWIW, I'll plan to rigid tap in my CNC mill in back gear. And mount it in a end mill holder with ground detents and two set screws.
Also this tap is a bottomming unit. Would taking the trouble to grind it into a standard tap make for a smaller tap force? I'll keep watching for a standard tap but would like to get going with this one. (A new tap is $200)
Try boring a hole in scrap aluminum and tap by hand, try to gauge the torque. My guess is that it will work easily on a decent hobby size milling machine like yours, because this is a fine thread.
If you are doing this in a CNC I would recommend thread milling it. It is a lot easier on the machine. I power tap A36 steel up to 1.5 inches but I have the HP and a big machine to push the tap. (Monarch VMC150) I have some 3 in. x 10 tpi threads to do next week as soon as they send me the right insert for the threadmill. The machine according to the spces. should drive the tap but threadmilling a big hole works so much nicer.
Make sure the motor is running in the high end of the rpm range so you get full hp out of it.
For power tapping, you want a gun tap (spiral point tap) which will chase the chips ahead, or a spiral flute tap, which will chase the chips back out the hole you come in.
The photo has been removed on that auction, and replaced with one just saying "Closed", so I can't look at the tap -- but if it looks like this one (1-1/24 16) in auction # 140451490510, it does not have the spiral point grind.
I'm not at all sure that you can get enough torque to tap using the back gears. For something this large, with a CNC mill, I would suggest that you get a thread mill instead, which mills the threads as you walk the mill around the hole in a spiral at thread pitch rate.
You've got CNC -- go for thread milling, not a tap. With a 1/4" hole, you may not have clearance for thread milling, but for a 1-3/16" threaded hole, you have plenty of room. You can either get a thread mill for 16 TPI, or a general single thread one which you can use for any reasonable thread pitch.
for what it's worth, I've had no problem tapping cold rolled steel with
1.25 inch tap in my mill, the trick, since it was a manual mill, was to have a holder that would let the tap advance at its own rate. I think I ran it at slow speed (45 rpm) and didn't see any bogging down of anything. I probably could have run much faster, but for one hole, what's the rush?
thread milling is my backup plan. I know I'd never hold the required specs on my old machine with a threadmill. I'd make it undersize and chase the thread to size with this tap. No way am I going to find this threadmill insert on the bay, so far no joy on the threadmill holder.
I'm a bit worried about bad things happening just trying to tap directly this big tap in a machine.
If you are doing 2B thread you should have no problem with holding tolerance with your machine unless you have a lot of backlash in the axis. Here is a thread mill that would work for your job.
formatting link
The tap you bought was listed as a special. ???? oversized? you better check what the special means. It should be marked on the tap.
Here is another thread mill with a smaller diameter which will make it easier for you to cut the thread. The larger one will work but it could give you chip clearance problems.
Why? How tight is the spec? How much backlash in your machine? (With ball screws, there should be very little.) The main thing is whether the mill has a helical canned cycle, since that is the motion you would need for thread milling.
I would too.
formatting link
Nope! Form the auction description:
CAN BE USED FOR A 1-5/16"-16 OR LARGER THREAD
and he is after a 1-3/16" thread, so this one is too big. If he does not need to do too many of these, a thread mill 1/2" diameter or so would probably do quite well.
Look at something like MSC item 81262487, which is a single thread and can cut pitches between 0.062" and 0.125" (and you need a pitch of 0.0625" for 16 TPI, which just barely eliminated the 1/2" diameter version. This one is 3/4" diameter and 3/8" diameter shank. Maximum cut length of 3/4". We're still talking about somewhere in the $90.00 range IIRC -- but that is new price -- and it will cover a wide range of thread pitches and diameters, not just the pitch and diameter you are after.
You first circularly mill the ID of the threaded hole, then you move the thread mill down the hole in a spiral, cutting your thread.
Your concern is well founded. Power tapping with a straight flute tap without a spiral end grind (gun tap) is asking for trouble, just as DoN suggested. Driving the tap isn't much of an issue (assuming you're tapping aluminum), but unless the hole is shallow, the flutes will pack almost instantly, resulting in a jammed tap. That's the reason you stop and reverse when hand tapping--to free the flutes of chips.
I do not recommend you attempt to alter the grind of the tap. While it's not impossible, the end result is often a tap that will no longer create a thread within acceptable limits. One flute will generally cause the tap to wing to some degree, cutting oversized.
PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here.
All logos and trade names are the property of their respective owners.