to Use Threadmills
To produce internal threads, drill the minor thread diameter
to its appropriate size. The, position the threadmill to the
required depth. Next, mill either the ‘X’ or ‘Y’ axis to the
required thread pitch diameter. With small sized and with
difficult-to-cut material, it may be necessary to remove the
material in several passes. It is always best to "arc-in"
and "arc-out" when threadmilling. Any "arc-in" and "arc-out"
movements must have a corresponding ‘Z’-axis motion during
the ‘X-Y’ circular moves. For example, if the "arc-in" is
over 90 degrees, the ‘Z’-axis departure must be ¼ of the thread
pitch. (90 degrees is 1/4 of a circle).
A right-hand thread is produced by orbiting
in a counterclockwise direction while bringing the ‘Z’-axis
up one pitch per 360 degrees. A left-hand thread is produced
by orbiting in a clockwise direction while bringing the
‘Z’ axis up one pitch per 360 degrees. The entire process
can be achieved by interpolating in a downward direction
and reversing the orbit direction.
External threads must have the major diameter
milled to size before the threadmill is used. Right-hand
threads are cut by interpolating up and in a counterclockwise
direction. The same threads can be cut by interpolating
down and changing the orbit direction.
NPT threads are usually produced while
interpolating the tool in a downward direction. Since these
tools are crest cutting, it is not absolutely necessary
to ream the internal minor diameter or mill the external
diameter to size. However, it is highly advisable to do
so since the tools will have much less material to remove.
If the tool is to be interpolated in an upward direction,
spiral interpolation must be used.
The same SFM can be used for threadmills
as for endmills of the same size. The feed rate must be
slower, however, since threadmilling often involves unfavorable
length-to-diameter ratios. Also, keep in mind that the threadmills
have more surface area contact than an endmill of equal
length. Most CNC mills are programmed in inches per minute,
which is applied at the centerline of the spindle. In internal
applications, the outside diameter of the tool will be traveling
faster than the centerline of the tool. The reverse is true
for external applications. It is best to start out conservatively
with feed rates and the number of passes required and adjust
upward per good machining practice.