Content Preview
TB029 Rev1 Thread Milling
Overview
This document describes the steps necessary to implement internal and external threading operations using a
CNC control capable of true simultaneous three axis interpolation such as the Centroid M Series CNC
controls In software versions v6 02 and later a thread milling cycle was added in Intercon This document is
intended for systems that have software versions prior to v6 02
Tools
There are two types of cutting tools to consider for threading operations One is the single point cutter which is
cheaper and more versatile than the second type the full form cutter which can save time when cutting
standard thread sizes When selecting a tool be sure to consider the minimum and maximum pitch the tool
can be used for as well as the diameter
Techniques for internal threading
The basic internal threading nuts technique involves the following steps It is assumed that a hole has been
bored with a diameter equal to the thread minor diameter and that a right hand thread will be milled
1 A rapid move to the center point of the thread
2 A feed to the depth of the thread if milling from bottom to top or a feed to the surface height if
milling from top to bottom
3 Turn on cutter compensation Use left G41 compensation if milling from bottom to top Use right
G42 compensation when milling from top to bottom
4 Move to a starting point on the arc defined by the major diameter of the thread The diameter of
the arc is equal to the thread major diameter for internal threading This value can be found in a
reference table such as that listed by Machinery?s Handbook For example an internal thread with a
one inch diameter has a major diameter of 1 0000" Any move to a point 0 5000" half of the thread
diameter from the center point of the thread is acceptable This move is typically a one axis move
and should not be an arc move
5 Perform a helical move This involves a 360 degree arc in the XY plane with a Z move equal to
the thread pitch and in the appropriate direction Use G2 CW arc if milling from top to bottom Use a
G3 CCW arc if milling from bottom to top
6 Repeat step 5 for the number of threads needed This can be calculated as thread depth in
inches time?s threads per inch
Techniques for external threading
The basic external threading bolts technique involves the following steps It is assumed that a cylinder of
proper height with a diameter equal to the thread major diameter exists and that a right hand thread will be
milled
1 A rapid move to a point outside the cylinder To achieve proper cutter compensation results make
the move to a point that is at least one half of the thread tool diameter from the cylinder that will be cut
2 A feed to the depth of the thread if milling from bottom to top or a feed to the surface height if
milling from top to bottom
3 Turn on cutter compensation Use right G42 compensation if milling from bottom to top Use left
G41 compensation when milling from top to bottom
4 Move to a starting point on the arc defined by the minor diameter of the thread This value can be
found in a reference table such as that listed by Machinery's Handbook For example a one inch
diameter thread with eight threads per inch has a minor diameter of 0 8492" Any move to a point
0 4246" half of the thread minor diameter from the center point of the thread is acceptable This
move should not be an arc move
5 Perform a helical move This involves a 360 degree arc in the XY plane with a Z move equal to
the thread pitch and appropriate direction Use G2 CW arc if milling from top to bottom Use a G3
CCW arc if milling from bottom to top
6 Repeat step 5 for the number of threads needed This can be calculated as thread depth in
inches time?s threads per inch
Additional Tips
1 For cases where the fractional part of thread pitch exceeds four digits it may be necessary to
calculate the absolute Z position for each thread and then round off as opposed to moving the Z axis
incrementally the distance obtained from rounding the pitch value to four digits at the start Rounding
the pitch from the start can cause errors that increase as the thread depth and number of threads per
inch increases
2 When using Centroid Shop Floor Programming SFP 360 degree arcs cannot be entered as an
EP&R end point and radius type Use the center point and end point type of arc CP&EP
3 When milling threads from top to bottom it may be possible to use Intercon's Repeat to Depth
Sub Program after the first helical is performed
4 For left hand threads reverse all the cutter compensation and arc directions
Document History
Rev1 Created on 1999 08 23