Novice Tapping in Aluminum Help

[NewCNCist]

I'm very new to machining, and the little experience I'm building is entirely centered around machining bisque fired and powder compact ceramics. That being said, I'm having a lot of difficulty machining aluminum (6061-T651).

I'm running a Haas TM-2P mill, with 6000rpm max spindle speed. I'm under the understanding that aluminum is generally machined at higher speeds than I'm capable of, and I have a copy of the Machinery's Handbook, but considering the results I've gotten trying to down scale parameters, using the book as a reference, to accommodate what my machine can do I'm clearly doing something (or a lot) wrong.

I've been trying to tap 1/4in-20 blind holes, a half inch deep, into predrilled 3/16in holes to no avail. I know that this isn't the ideal starting hole, but I figured since my work does not need to be precise that this would be workable. Am I wrong? Could someone please help me with a walk through (particularly feeds and spindle speeds that are possible for me??)?

Further info: I've shattered carbide core, TiN coated taps attempting this; am running under flow hydrolubric coolant; managed to produce one hole...but feed/speed was clearly off (produced a clean hole); any additional info for traditional surface milling is appreciated too, as that is what I will be doing next

 

[MiketheEngineer]

Tapping at 6000 rpm - I don't think so - but I am not an expert in this field.

How about trying 2 rpm and work up from there

 

[MikeHalloran]

You may be able to tap at 100 rpm, or the machine may have a canned cycle for it, but maybe you need to start by tapping a few hundred holes by hand until you understand how it works.

The proper tap drill for 1/4-20 is #7, or about .201".
OF COURSE a .1875" hole is going to break taps.

Buy a Machinery's Handbook and READ IT.

At least read the manual for the Haas machine; it has to cover some basic machining topics.




Mike Halloran
Pembroke Pines, FL, USA

 

[imcjoek]

In my limited experience, 6061 tends to machine like gummy bears.

Needs a lot of "chip break" cycles when tapping it. It is not uncommon to use #6 or even #5 as the tap drill. Usually you still get damn near 70% thread.

Also a thread FORMING tap will require a larger pilot hole than a standard cutting tap. Make sure you know which you are using.

 

[berkshire]

NewCNCist
Like imcjoek says 6061 is a little gummy to machine.
I would recommend that you use a thread forming tap for your blind hole so that you do not have to deal with the accumulation of chips. A #1 drill will give you 65% thread
B.E.

The good engineer does not need to memorize every formula; he just needs to know where he can find them when he needs them. Old professor

 

[moldmaker1001]

NewCNCist,

First, if I was using a tap, carbide would not be my first choice,

A good quality HSS or Cobalt with TiAn Coating works well. I

would start with a #5 Tap drill, make sure you are drilling deep

enough, to avoid chip packing. I would run that tap at 300 RPM,

which would give you a feed of 15 in/min.

 

[Eltron]

The minor diameter for a 1/4-20 thread is 0.1876". Your tap drill is 0.1875". See a problem there? Generally you can shoot for 75% threads on aluminum. The formula for tap hole size based on thread % is: Tap Hole Size = Basic major Diameter - (1.08253 * % Full Thread)/Threads per Inch.

Dan

http://www.eltronresearch.com

Dan's Blog

 

[BillPSU]

The first problem you are having is the tool you are using. You stated this is a blind hole meaning the chips have to be pulled out of the hole. The best tool will be a fast spiral polished flute tap. Now you have to decide what chamfer to use, bottoming 1-2 threads, plug 3-5 threads or taper 7-10 threads. That depends on how deep you drill the tap drill. I would drill the hole .75 deep full diameter or .82 deep to the point and use a bottom chamfered tap. 300 RPM is a reasonable speed for tapping and use either a water soluble coolant or cutting oil suitable for aluminum.

Your problem with tapping was probably you were using a spiral point tap or a hand tap and clogging the hole with chips and breaking the tap. Also when tapping you are reversing the spindle direction and depending on the rpm the gear train of the machining center has inertia and reversing does not happen quickly enough and the tap bottoms in the drilled hole.

 

[ornerynorsk]

First things first, is your machine equipped with rigid tap and are you using/programming it correctly? Double-check your feedrate/rpm calculation.

A 3/16 hole is too small, as others have mentioned. That alone will break taps.

As Billspu said, you will need a fast spiral tap to pull your chips (strings, rather) out of the hole, and allow extra hole depth for tap end clearance. 300 rpm is pretty slow, you should be able to double that and use a P retraction factor of 1.25 to 1.5 to help speed up your cycle, ONCE you have figured out the initial problem.

Good luck.

It is better to have enough ideas for some of them to be wrong, than to be always right by having no ideas at all.

 

[unclesyd]

Adding to the information posted above the use of a proper lubricant is essential regardless of the thread form. We have had great sucess using the product Tap-Magic for Aluminum.

Another thing you might want to consider if the quantity is there is to use a tapping head on your machine. This will give you the optimum production and save a lot of taps and tapped components.

http://www.steco.com/TMaluminum.htm