TECHNICAL INFORMATION

WORKPIECE
MATERIAL

Specific
Grades

Speed
SFM

FEEDRATE (inches/tooth)
Tool Cutting Diameter

1/8

3/16

1/4

5/16

3/8

1/2

5/8

3/4

Low Carbon and Leaded
Steels <25Rc

1005-1029
12L14

550
"

0.0003

0.0006

0.0001

0.0013

0.0017

0.002

0.0027

0.0035

Medium Carbon and
Alloy Steels 25-35Rc

1030-1050
4130, 4140, 4340

450
"

0.0003

0.0006

0.001

0.0012

0.0015

0.0018

0.0025

0.0032

Medium Carbon &
Alloy Steels 36-46Rc

1040, 4130, 4140
4340, 52100

250
"

0.0003

0.0004

0.0007

0.0009

0.0012

0.0015

0.002

0.0025

Aluminum Alloys

6061, 6066

1200

0.0004

0.0008

0.0012

0.0017

0.0021

0.0025

0.0035

0.0042

Brass

Free Machining

1000

0.0004

0.0007

0.001

0.0015

0.0018

0.0022

0.003

0.0037

Titanium and
Titanium Alloys

Commercially Pure
6AI4V

350
250

0.0003
0.0003

0.0005
0.0004

0.0007
0.0006

0.0009
0.0008

0.0012
0.0011

0.0015
0.0013

0.0021
0.0018

0.0028
0.0022

Nickel Alloys

Inconel 718, Waspaloy
Hastelloy
Monel 400 series
Monel 500 series

80
100
200
140

0.0003
0.0003
0.0003
0.0003

0.0004
0.0004
0.0006
0.0004

0.0005
0.0005
0.0008
0.0006

0.0007
0.0007
0.0001
0.0008

0.0009
0.0009
0.0013
0.0011

0.0012
0.0012
0.0018
0.0015

0.0016
0.0016
0.0022
0.002

0.0022
0.0022
0.0028
0.0025

Stainless Steels

300 series
400 series
15-5PH, 17-4PH
Nitronic 32,33,40,50,60

350
400
250
150

0.0003
0.0003
0.0003
0.0003

0.0004
0.0004
0.0004
0.0004

0.0006
0.0006
0.0006
0.0005

0.0008
0.0008
0.0008
0.0007

0.0011
0.0011
0.0011
0.001

0.0015
0.0015
0.0015
0.0014

0.002
0.002
0.002
0.0018

0.0025
0.0025
0.0025
0.0022

Cast Cast Iron

Gray
Ductile
Malleable

500
425
400

0.0004
0.0005
0.0004

0.0006
0.0007
0.0006

0.0009
0.001
0.0009

0.0011
0.0013
0.0014

0.0014
0.0017
0.0014

0.002
0.0025
0.002

0.0028
0.0032
0.0028

0.0035
0.004
0.0035

Tool Steels

H10, H12, A2
D2

325
225

0.0003
0.0003

0.0004
0.0004

0.0007
0.0007

0.0009
0.0009

0.0012
0.0012

0.0015
0.0015

0.002
0.002

0.0024
0.0024


When cutting an internal thread the linear feedrate has to be reduced to compensate for the ratio of the tool's cutting diameter to the major diameter being cut.  If you do not compensate, the feedrate that the cutting edge sees will be much greater and tool failure will occur. The threadmilling feedrate is equal to:

((major diameter - cutter diameter)/major diameter) x linear feedrate

Example #1
Thread Diameter to be cut (D2):  3/8
Threadmill Diameter (D1): .285

If the linear feedrate calculated from the feeds and speeds above came out to be 10 IPM the programmed feedrate for the internal threadmilling cut would be: ((D2-D1)/D2) * linear feedrate  or ((.375-.285)/.375)*10  or  2.4 inches per minute

Example #2
If you were going to cut a 1/2-13 thread in a low alloy steel that was less than 25 Rc hardness:

 Question: Which tool would you use?
Answer:  #TM50013 which has a .350 cutter diameter and 4 flutes

Question: What surface speed should you run?
Answer: 350 - 500  (We will use 400 SFM) 

Question: What is the chipload per tooth?
Answer: .0025-.0035 per tooth (We will use .003"/tooth)

How do you calculate RPM's?  
Take 3.8 divided by the threadmill dia and multiply by the SFM
Example: ((3.8/.350) * 400 SFM  = 4343 rpm

How do you calculate linear inches per minute? 
Take the ("/tooth) * (# of flutes) * RPM's
Example: ((.003" * 4 flutes) * 4343 RPM's = 52 linear "/min

What will be the programmed feedrate when cutting a 1/2-13 internal thread?
Answer:((D2-D1)/D2) * linear feedrate or  ((.500 - .350)/ .500) * 52 ipm = 15.6 IPM