Phone:1.508.754.1198 | Toll Free:1.888.754.1198 About Us
Privacy Policy


Kipware Real World Software
Follow Us on Facebook    Follow Us on Twitter

Stop Scratching Your Head and Make Some Chips !!

Shop Formulas That Make Everyone Productive

You perform important calculations every day, perhaps every hour, that make the difference between productivity and helpless floundering. Two points need to be made :

  • Do you know the right Calculations?
  • Do all your shop floor compatriots?

This article will outline some of those important formulas for your use and for you to pass out to your fellow shop floor friends. Print this page from your Browser, Keep it close, inside your favorite shop book or your Machinists Handbook and we guarantee you'll find yourself and your shop doing less HEAD SCRATCHING and more CHIP CUTTING

If you want an easier way to get these calculations done and many, many more, check out our KipwareTB Software. KipwareTB will do these calculations quickly and accurately, all in the simple WINDOWS environment so anyone can do them. Just put KipwareTB on your shop floor PC and watch the difference in productivity. Click the link below to check out KipwareTB.

KipwareTB Logo


Click the Formula Desired or Browse the Page :

IN -- MM Conversion

The formulas below are to convert a IN dimension to MM and vice versa.

  • MM = inch x 25.4
  • IN = mm / 25.4

SFM -- RPM Conversion

The formulas below are to convert a Surface Feet Per Minute (SFM) speed to straight Revolutions per Minute (RPM) and vice versa. DIA is the DIAMETER of the workpiece for a Lathe or Turning calculation or the TOOL DIAMETER when calculating for a milling machine.

  • SFM = ( RPM x DIA ) / 3.82
  • RPM = ( SFM x 3.82 ) / DIA

Drill Point Length Calculation

The formulas below will calculate two dimensions commonly required in the Real World.

  • How deep to go with the countersink to get a specific diameter
  • How deep to drill to clear the tool tip through the part.

In the formula, DIA is the total tool diameter ( 1/2 drill = .500 ) and ANGLE is the TOTAL angle that the drill point is ground. A normal twist drill is about 135 degrees. As you can see, we divide both in half so radius values can be substituted and the formual altered as appropriate.

  • Depth = ( DIA / 2 ) / TAN ( ANGLE / 2 )

IPR -- IPM Conversion

The formulas below are to convert an Inch Per Revolution (IPR) speed to an Inch per Minute (IPM) and vice versa. You can use (1) as the number of teeth when calculating turning speeds.

  • IPM = ( # of teeth in the cutter x IPR ) x RPM
  • IPR = ( IPM / RPM ) / # of teeth in the cutter

Cutter Comp Shift Calculation

Anyone who has programmed any turning for chamfers or radii knows how important the Tool Nose Radius (TNR) is in making the correct chamfer or arc cut. Most times, the machines cutter comp feature can be employed and the problem solved, however, sometimes not so easy. The formulas outlined below are for the perfect 90 degree intersecting examples as shown in the graphic and will calculate the actual tool shift amount to manually compensate for the TNR when cutting chamfers and radii of that type. You can do these calculations and adjust the start point and end point accordingly to compensate for the TNR quickly and easily and without the use of the machines Cutter Comp feature.

As stated, the formulas below are for chamfers and radii as outlined. X value is a DIAMETER values, divide it in half if your machine uses RADIUS programming in the X axis. Where and how to apply the calculated shift amounts is shown in the graphic.

Cutter Comp Shift Examples
  • Compensation for an Angle

    Z Shift Amount at the End Point = TNR x ( 1 - TAN (ANGLE / 2))
    X Shift Amount at the Start Point = ( TAN (ANGLE) x Z (above)) x 2

    When employing these values, move your calculated start point by the X value above and the Z end point by the Z calculated value above.

  • Compensation for a Radius

    Z Shift Amount at the End Point = TNR + Part Radius
    X Shift Amount at the Start Point = 2 x (TNR + Part Radius)

Thread Depth Calculation

The formulas below cover both Internal and External, standard 60 degree threads and will calculate the recommended depth of the thread. Depths calculated are Per Side depths to be used when determining the diameter to be programmed in the thread commands.

  • External Thread Depth = .61343 x ( 1 / # of threads per inch)
  • Internal Thread Depth = .54127 x ( 1 / # of threads per inch)

Disclaimer : CNC TIPS are provided without charge or obligation by Kentech Inc.. It is the responsibility of the reader to perform any action outlined here in a safe and responsible manner. The reader assumes all responsibility for service or actions taken as a result of the information contained here. KENTECH INC. and its employees assume no responsibility for personal or property damage, any type of monetary losses or losses caused directly or indirectly from the material provided in this Web page or any pages contained in the WebSite.

THIS DISCLAIMER OF WARRANTY AND LIMITATION OF LIABILITY IS GOVERNED BY THE LAWS OF THE COMMONWEALTH OF MASSACHUSETTS

Back to Tips Page