Hey guys, I need to tap a bunch of 2-56 holes in 6061. .3 deep, blind holes. I have generally been tapping (rigid) at 1000rpm using spiral flute taps (mainly 1/4-20 and 10-24). I dont have much experience with such small holes. What do you recommend as a good place to start?

Thanks

Mark

Are you considering forming taps or spiral flute? You know the difference between the four types, right?



Hand taps: straight flute and don't eject the chips anywhere. No good for machine tapping.
Spiral point: eject the chips out the front of the tap (into the hole). They only work with very deep holes or through holes.
Spiral flute: eject the chips along the axis and out the top. The spiral flutes make the tap weaker.
Forming: no flutes at all. Uses a slightly larger drill size and actually forms the threads by deforming the metal. Strongest because they have no flutes. Good choice in small sizes like your #2 holes.

Sorry if you knew all of that. I had to learn the subtleties between my choices before I finally stopped breaking taps. :withstupi

sometimes you need to be careful when it comes to what type of tap to use in regard to cutting or roll taps , there are many cases where customers will not take a part if it has been form tapped but generally it will be specified by the customer before hand

in general on a 2-56 I would prefer to use roll taps

I had to tap 216 holes to a depth of .4 in these wheels...

http://i15.photobucket.com/albums/a353/ShyGecko/RD400/JIAsfinishedwheels002.jpg

http://i15.photobucket.com/albums/a353/ShyGecko/RD400/JIAsfinishedwheels005.jpg

For 2-56 x .375 SS bolts
http://i15.photobucket.com/albums/a353/ShyGecko/RD400/JIAsfinishedwheels009.jpg


Using a spiral flute at 1000RPM. The coolant was rich (about 15%). no taps were hurt during the making of these parts....

If you use a spiral flute tap, then I would recommend that you turn on 'repeat rigid tapping' in your Haas, and tap the hole in 2 or 3 steps (progressively deeper).

I would also use a tapping fluid specifically for aluminum.

Be sure to check (running the program without a part in place) how far the tap overruns in the Z travel before it reverses direction. My VF3 (1996) usually runs about .05" extra so allowance has to be made for that in commanded thread depth, or in extra drilled depth.

Running those little taps is a bit un-nerving, the first time through, on blind holes. You just double check everything, and then clench your teeth and press the button. :D

If you have a geared head, make sure to override the speed change (use M42 to stay in high range) if running below 1500 rpm. There is less momentum for the motor to stop, and thus it will stop faster for reversals.

Thanks a lot for the input guys.

Greg, I used to use only spiral flute taps and then started form tapping for the 1/4-20 and 10-24 holes I do a lot of. I was going to use spiral flute on the since I have them already but maybe as dertsap suggests I will use roll taps. Is there a table online that someone knows of that I can download a table that suggests the correct drill size for roll tap?

Thanks

Mark

http://www.4hiretek.com/tapdrill.html

thanks a lot dertsap