Keep Breaking Taps

[Crashmaster]

I am tapping with a 10-32 tap on my Wasino lathe and keep breaking the damn thing. Just wondering what types of taps people have had success with on cnc lathes. I am tapping 12L14 which makes this even more frustrating.

[Karl_T]

OSG taps are my fav. brand. Many other good ones.

If you're breaking a tap in 12L14, i suspect something wrong in your tap cycle. This stuff is like butter to tap.

Karl

[Crashmaster]

I'm pretty sure the tap cycle is ok. I can run 50ish parts on the tap before it breaks. However, the last time I ran this program (over a year ago) I was kicking out 500+ parts on one tap. The problem is that we probably are using different taps then we did a year ago, but I'll be damned if I know what type/brand they were. I'm on my way to pick up a few helix cut 3 flute bottoming taps. We'll see if they are more successful.

[msomerville]

I agree with Karl. Unless you are bottoming out against chips I think the problem may lie in the tap cycle. Have you ever tried thread roll form taps? The reason I like them is that is forms the threads and doesn't cut the threads thus no chips in the bottom of the hole. It is a stronger thread too.

[Crashmaster]

With thread roll form taps, do you undersize the hole?

[mactec54]

Hi crashmaster

The roll form taps use a bigger drill 10-32 is a number 16 drill
this is for 65% thread you can play with this drill size a little
to get the thread fit you want

[stupidog]

Have you checked the turret alignment?

[IslandLad]

10-32 UNF (I gather thats the thread form?)
You don't say if the hole is blind or through?
Spiral Flute and Spiral Point taps require a 4.1mm drill.
Thread Former (Roll taps) require a 4.45mm drill.
Make sure you are using the correct cutting data for the material and drill type. If you are not using the right speed & feed you can cause the drill to rub more than cut, which creates a hard surface. Then the tap will have a harder time cutting the thread. What drills are you using? With this material you shouldn't need to drill a slightly bigger core hole, this normally applies to Stainless Steel, Titanium etc.
Insure you have plenty of coolant and that the mix is correct. Try increasing the percentage of emulsion to 10%.
Have you checked the Cutting speed of the tap? On a good quality tap you should be running at 10-20m/min. High performance taps will run quicker.
Are you rigid tapping? If you are a sufficiently large clearance distance should be programmed. If the distance is to small there is a possibilty that the machine is not synchronised with the feed before entering the hole.
You also need the check for chip clogging.
Breakage could also be caused by cutting teeth overload. Use a tap with longer chamfer. Increase the number of flute if possible to obtain more cutting teeth.
Check the angle and position of the core hole. If the work piece is not clamped properly then the tap maybe trying to tap a hole that out of position. Use a tap chuck with axial floating.
Your tap could be bottoming out. Drill deeper than the required thread depth. There could also be swarf in the bottom of the hole. This is likely if you are drill pecking. Try using a drill with a split point (self centre) that is designed to drill without pecking. A drill with wide flute to give enough space for swarf to travel down the flute freely.
Another solution would be to use a tension & compression chuck. There are two main types. On machines that the feed cannot be programmed to match the pitch, taps are best use with a chuck that has intergrated length adjustment. This compensates for the difference between table feed and tap pitch. The slow down of the spindle at the reverse point of the threading cycle is compensated. 12mm movement under tension & compression. Modern machines are designed so that the feed match's the pitch. The feed and spindle speed are synchronised. Machine manufacturers like to promote this as the be all and end all. But its not. In the real world the dynamics of the linear drives produce syncronisation errors, especially during the tap reverse. Special taps designed for CNC rigid tapping might help as they are designed to cope with the axial stresses produced by this process. The second type of chuck is designed for rigid tapping. They have a minimum length adjustment under tension & compression (1mm under tension & 0.2mm compression). This increases the tool life by reducing the axial force on the thread's flank.
Look for taps with a minimum of stream tempered to improve the surface hardness and reduce surface friction.
I hope this helps???