What's new
What's new

Roll Form Tap vs Cutting taps Looking for thread forming that requires low torque

mikemxparts

Plastic
Joined
May 27, 2022
I am running an M17 1.5 tap in aluminum at .500" depth. My Kitamura Mycenter1 does not have enough torque to spin the tap unless I bore the hole oversize. My question is: Does Roll Form Taping require more or less torque than cutting taps? Also if taps require less torque what type tap requires the least torque?
 

Vancbiker

Diamond
Joined
Jan 5, 2014
Location
Vancouver, WA. USA
I am running an M17 1.5 tap in aluminum at .500" depth. My Kitamura Mycenter1 does not have enough torque to spin the tap unless I bore the hole oversize. My question is: Does Roll Form Taping require more or less torque than cutting taps? Also if taps require less torque what type tap requires the least torque?
What RPM are you tapping at? If too low you might be successful with more speed to get into the power curve of the machine. IIRC, the Mycenter1 had a few different spindle speed options. What is on your machine?
 
  • Like
Reactions: Ox

Doug

Diamond
Joined
Dec 16, 2002
Location
Pacific NW
As to what form tap require the least torque..... the best form taps I've found have a 4 lobe cross section with the 4 lobes in a helix up the tap. I have no way to measure the required torque. All I can say is with tapping many thousands of 12L14 holes 10-32 by 7/8" deep I had far less tap breakage with those.

The absolute worst form taps for me were Balax with a pressure relief groove up the side. While thread forming is in theory a chipless operation you still get swarf which can plug that relief groove leading to tap breakage.

Something to watch out for with form taps. After long use they can wear diameter-wise on the first few turns at the tap end leaving undersized threads at the bottom of the hole. It's important to verify the threads all the way to the bottom with a gauge. When I retired my customer bought 5,000 parts from another shop, everyone had bad threads in the last 1/4".

A trick in a pinch.... Form taps sometimes break off on the end. Always seemed to happen when it was our last tap. My first thought was to grind a nice end chamfer on the T&C grinder. Then I found you could do the chamfer by hand just spinning the tap in your fingers on the bench grinder.
 

prime_mover

Plastic
Joined
Jul 3, 2017
Taps with a longer chamfer length require less torque, which is to say a plug tap will require less torque than a bottoming tap. The best taps for aluminum are the GLT8 (DLC) coated taps by EMUGE. The best taps are made by Emuge, period. They don't make an M17x1.5 tap though. If you are applying lube, Relton A9 works good and is non-toxic. Other than that: thread milling.
 
Last edited:

mhajicek

Titanium
Joined
May 11, 2017
Location
Minneapolis, MN, USA
In aluminum you can run a pilotless threadmill in a competitive cycle time to drill and tap. There are some designed to mill the pilot while threading, and others that are combo drill/threadmill.
 

BT Fabrication

Stainless
Joined
Nov 3, 2019
I am running an M17 1.5 tap in aluminum at .500" depth. My Kitamura Mycenter1 does not have enough torque to spin the tap unless I bore the hole oversize. My question is: Does Roll Form Taping require more or less torque than cutting taps? Also if taps require less torque what type tap requires the least torque?
for that, you would need a 15-20 hp motor and really low gear reduction to turn that one.
if its a small machine with a 7.5 or 10 hp, you wont cut it either way. as it needs something like a 3/4-10 that is 7.98hp before any gear box hp losses.
 

Conrad Hoffman

Titanium
Joined
May 10, 2009
Location
Canandaigua, NY, USA
Yeah, 17 mm is 0.67" and I could run that form tap in by hand (in aluminum) with a decent tap wrench, and I'm not producing very many HP these days! Now, there's the question of how fast you want to do it.
 
  • Like
Reactions: Ox

DavidScott

Titanium
Joined
Jul 11, 2012
Location
Washington
What RPM are you tapping at? If too low you might be successful with more speed to get into the power curve of the machine. IIRC, the Mycenter1 had a few different spindle speed options. What is on your machine?
I think my 2001 version with a 10 hp Yasnac motor switches "gears" at 3750 rpm, or really close to that. It has a two speed motor. The book says M24x3 in S45C with a minimum spindle speed of 150.
 

mikemxparts

Plastic
Joined
May 27, 2022
On our Fadal we use thread milling but this Kitamura has a Fanuc 3M control and does not do 3 axis interpolation so I am limited to tapping. I need a newer machine !!
Yeah, 17 mm is 0.67" and I could run that form tap in by hand (in aluminum) with a decent tap wrench, and I'm not producing very many HP these days! Now, there's the question of how fast you want to do it.
I can't find a form tap for M17 x 1.5
 

mikemxparts

Plastic
Joined
May 27, 2022
What RPM are you tapping at? If too low you might be successful with more speed to get into the power curve of the machine. IIRC, the Mycenter1 had a few different spindle speed options. What is on your machine?
I was tapping at 260 rpm. I didn't know the machine would have more torque at higher rpm's. It is a 1984 Mycenter1 Fanuc 3M dripfeed 8000 rpm max spindle, no gear box
 

FamilyTradition

Aluminum
Joined
Feb 24, 2018
Location
Greenfield, Mass
I haven't done much thread milling myself, so I can't speak to that. However, someone close to me works for a large company that makes taps, and suggests that you check to see if the taps you are using have any radial relief. This may help with your torque problems - a lot of taps they produce have no relief on the lands, and such rub a bit all the way down. They've seen radial relief work wonders in certain applications.
 








 
Top