cutting taps

[anderslr]

I'm looking for a industry standard for cutting tap depth. I want to finish the tapping on a CNC machining center with no hand tapping. I have heard 1.5 x diameter would be reasonable.

Thanks in Advance

 

[ornerynorsk]

There is no industry standard. You need to have the part do what it is intended to do. I can tell you that once you go past 2X diameter on the depth, tap breakage will increase on blind holes. Through holes don't seem to be a problem.

 

[Philrock]

The required depth should be on the print. If it's not on the print, ask. If you can't get an answer, I'd suggest 2X diameter. As ornerynorsk says, ther is no standard. Since the tapped material is usually softer than the fastener, 1.5 diameters is minimal engagement. The fastener could be too short for 1.5 diameters engagement. 2 diameters gives a little more leeway.

 

[psychomill]

Small taps may be in the range of 3-6D, larger (say 3/8 or so and up) may be at 2-4D. As others have said though, this not set in stone. This will change with different makes, type styles etc. 1-1/2D shouldn't be a problem at any size (unless you're tapping a 2" thread - then its a HP issue).

 

[BillPSU]

In mild steel the rule is 1.5 x the diameter for thread engagement so tapping 2 x the diameter is easily accomplished. Up to 3 x diameter is not too difficult, but watch your minor diameter and consider less percentage of thread if tap breakage becomes a problem. Increasing the tap depth will increase the cutting torque and tap breakage. Through holes are easier to tap as the chips can be pushed out of the hole with a spiral point tap. Blind holes should be tapped using spiral flute taps with the longest allowable chamfer. I have tapped up to 5 x diameter through hole but used a spiral point nut tap with interrupted threads. The interrupted thread reduces the drag of the trailing threads.

 

[unclesyd]

BillPSU's post is right on target as to the use of spiral taps and not tapping normal thread depth. We use both approaches to tap some very deep holes in Austenitic and Precipitation Hardening SS. As stated above we can also get a 5 with relative ease, anything else is an nail biter. Keep the Elox handy.

You need to work with your tap vendor and try different companies taps. We have found that there is sometimes a significant difference in a particular style between companies. We also saw a difference in performance based on different types of the coatings by and within each manufacturer. Along with different coolants not all the coatings behave the same.

One thing in machine tapping is that the deeper the tap the better the hole has got to be. The closer to round the better.

 

[JDana]

We recently ran a prototype order roll-form tapping 6-32 through holes in aluminum .900"+ thick.