Need help with 1/4-20 Thread mill on 304SST

[Tinhman]

Guys,

I am having a problem with 1/4-20 thread mill (.47 depth) on 304SST.

Tool use is Scientific TM170-20HA with 9 active teeth.

Please help.

 

First tried:

S3400

F10.

5 rgh passes (.005 per pass)

2 finish pass, step over .001

1 spring pass

Tool broke at the first hole

 

Second tried:

S1400

F2.

7 rg passes (.003 per pass)

2 finish passes

1 spring pass

Tool broke at the thrid hole.

 

Down to the last tool now.

What could be wrong here and what esle could i try??

 

 

Any input will be a big help.

 

Thanks.

[Pilot Plant Supervisor]

I don't have any experience with that type of thread mill, but I'll tell you what works for me. I use Micro 100 solid carbide thread mills that have multiple teeth on one plane, and I cut the hole right to size using cutter comp so I can sneak up on it. In Stainless and Titanium, I usually add a spring pass. I run 200 SFPM in Stainless with .0002 - .0005" per tooth feed. In Titanium I run 120 SFPM with the same feed.

[mkd]

inconel expert i know say they drill (Guhring carbide) a bit larger than 75% thread. a few thou on a 4-40 does make a difference.

waddaya drill to? with?

 

304 sucks

 

9 active seems to be a problem in my mind. too much cut force, not enough bending strength.

[Millertime]

inconel expert i know say they drill (Guering carbide) a bit larger than 75% thread. a few thou on a 4-40 does make a difference.

waddaya drill to? with?

 

304 sucks

 

9 active seems to be a problem in my mind. too much cut force, not enough bending strength.

 

+1

way to much cut force.We cut alot of 304 ss and do alot of threading using scientific t-mills with three active teeth.might want to try threading the hole in two depths.At a 120 sfm and .0009 fpt coolant flood

[Tim Johnson]

I don't have 304sst speeds but I run our 1/4-20 thread mill (VARDEX HC25192L05-I20UNF TM VTH) in 316sst s6560 F2.6, 1 pass. One tool will do hundreds of holes here.

[left coast lefty]

How are you drilling the holes? Maybe they are work hardened, or maybe they are close to a welded area? We use Scientific threadmills with 4 teeth, last month did 200 4-40 holes in titanium with 1 tool.

[EX-wccprogrammer]

This is a threadmill calculator from Carmex. Your tool should run similar.

[EX-wccprogrammer]

Carmex recommends bottom of hole out, one pass at a programmed rate of F2.2 for this thread.

[EX-wccprogrammer]

Here is a link to Carmex Calculator for those in need.

 

http://212.143.213.130/ToolRecommed.aspx (Threadmill Calculator)

[EX-wccprogrammer]

Allied calculator recommends this:

 

3 passes might work better in your case.

 

Both brands recommend feed around F2.2 or so, with RPM 6000 to 9000

[EX-wccprogrammer]

Here is a link to Allied threadmill calculator:

 

http://www.alliedmachine.com/Technical/ThreadMill/TM_Main.cfm

 

Note -- you do not have to fill in the information at the the top to use it.

 

HTH

[Tinhman]

Thank you guys.