tapping M2 x .4 blind holes

[Hash01]

I am using a 1998 okuma cadet mate with an OSP700M. Tapping blind holes in 6061 alm. It seems like it will run good for awhile but then starts snapping taps. Runnig a regular g84 cycle and in g95 mode. I was wondering if there was any helpful hints out there. Is there any way to dwell before backing out of the hole or peck tapping. Any suggestions are welcome.

[78nova]

What kind of tap are you using? Spiral or straight flute? What brand?

Are you using a floating tap driver?

What rpm & feedrate are you using?

I am not familar with M2 x .7 threads.

What is the diameter & pitch of the thread in inches?

What coolant or tapping fluid is being used?

Is a Cadet a lathe?

Why use are you using a G84 & a G95?

I tap as small as a 4-40. The normal speed & feed for this tap would be 400 rpm @ 10 ipm but we run @ 200 rpm @ 5 ipm, using an OSG fast spiral bottom tap with oil and a soft pressure floating holder.

[Hash01]

Sorry guys. It was a late night after a double shift and I wasn't thinking very good. It is an M2 x .4 straight plug tap. From what I can tell G84 is the only rigid option I have and G95 is in/rev to give better feed control. It is in a ER16 collet with flood coolant. This is on a 4020 mill. The tap is about the same as a 2-56 but a little finer more like 63.5 tpi. Thanks

[78nova]

OUCH! That is a very small thread and very easy to break but I would certainly try using a spiral flute tap to help evacuate the chips and make sure your minor diameter is up on the high side.

[Algirdas]

I would say M2 or M1,5 is small thread.
All depends on proper technology. Taping fluid is important for aluminum.
The main suggestion: use taping cycle without floating holder.

[JimF]

In my experience 6061 is a little gummy and, especially with such a small thread, the taps would be prone to break. Try a roll tap. They're flutless(or almost so), so they're stronger than conventional taps. You can drill the minor diameter larger than you would with a conventional tap, you will have to get the proper size from your distributor. The tap will then displace the material, yielding the proper minor diameter provided you have the correct size prior to tapping. A good roll tap will give you superior tool life and a stronger thread because the material is formed. Also, when programming the feed and speed of the tap, I don't know what your max RPM is for rigid tapping but a good start point would be around 1000 RPM with a feed of 15.75 IPM OR .01575 IPR. On a .4MM thread, the feed would be 15.748 IPM or .015748 IPR but most machines won't go to three places in IPM or six places in IPR feeds. This should still be OK because the difference will only be 2 millionths on the lead and I'm sure your length of thread isn't going to give you a problem with that difference.
If you can't use a roll tap, then you must at least get a good spiral flute tap, like someone mentioned below. Also, keep the toolholder you have. For rigid tapping, I prefer something solid rather than a floating holder.
Good luck!

[OkumaWiz]

I agree with JIMF, use a rigid holder and also sync tapping. Form thread it rather than cut threading. If you are running in inch and trying to do a metric thread, program the IPR @ .7/25.4 in your program in order to get a more accurate feed rate...yes they can do the math for a feed rate down to smaller than what is displayed. You may also want to keep your RPM below about 3000 RPM.

Best regards,

[Superman]

Another ditto about the roll taps, they are stronger.
your drill should be about 1.80/1.85mm (0.071/0.073") but check the specs and aim for the upper limit to lessen the power needed.

The only problem I can see is the use of G84, as this is a soft fuzzy type of cycle where the feedrate and spindle RPM are not accurately locked in sync and problems crop up when the spindle is reversed to come out, so you may have to use a floating tap holder and program the feedrate at 95-99% of the pitch ( breakages happen if using the higher RPM's )

Find out if G284 is available on your machine , this is normally the syncronized tapping cycle

Also use the G95 before the cycle, then you can alter the RPM anytime and not have to adjust the feedrates for all tap cycles

ie

G15 H_
G0 X_ Y_
S1000    ( G84 and G284 actually forces the spindle to start at the R-plane )
G56 H_ Z1.
G71 Z0.1
G95  ( unit / rev )
G284 Z-0.2 R0.1 F0.0157 M53    ( F= thread pitch )
X_ Y_
G0 or G80 ( cancels the cycle )
(G80 usually forces the spindle to stop, G0 keeps it going for the next operation)
G94  ( put it back to units / minute )( this is a must )