Thread milling
Thread creation is such a diverse topic. Over the past few months we’ve been discussing tapping. Now let’s take a look as threads from another perspective – milling. There are many advantages of thread milling.
The thread milling process requires a CNC milling machine with the ability to perform helical interpolation. In other words, to simultaneously control the X, Y, and Z-axis of movement at the same time. Not all CNC machines can do this.
Remember the challenges of using a tap and you’ll start to appreciate the advantages of the milling process. Tapping is a high stress operation with an overriding fact -- the feed per revolution of the tap must match the pitch of the thread we are producing.
Let’s review some of the challenges of tapping and compare some advantages of thread milling.
Problem with tapping: Tapping to full depth
This is a problem due to the chamfer on the tap and the clearance in the pre-tapped hole required to accommodate that chamfer. A tap may force the chips into the bottom of the hole, which can then cause the tap to break. With thread milling, it is possible to position the cutter to full depth and thread out of a hole, moving away from the chips, not into them.
Tapping feed rates
Our options when tapping are to vary the cutting speed of the tap or use a different type of tap, such as a cut tap or a form tap. Whatever method we select, we are still forced to program a Z-axis feed that must match the pitch of the thread.
Just compare the feed of a drill to that of a tap. We can feed a drill at whatever feed rate we select. For example a 3/8 - 16 TPI thread will use a 5/16 drill at 0.003 - 0.004 feed per revolution. The tap must feed at 0.0625 per revolution.
Thread milling feed rates
The thread milling process requires that we “ramp-in” to the full depth of the thread, produce one full circle and “ramp out” of the cut. During the full circle move we must move the Z axis a distance of one full thread pitch.
The feed rate of a thread mill is based on how quickly the cutter moves around the circumference of the part. One full circle will move the same distance of the thread pitch but how fast we move along this circle can be whatever feed rate we wish.
In tapping, the feed rate must match the thread pitch, in thread milling the cutting feed rate can be whatever feed you require.
Problems with tapping: Tapping cutting speeds
The majority of taps are made from high speed steel. Carbide taps are expensive and in some cases the brittle carbide can quickly breakdown under the high stresses found in tapping.
In our example we will use a single flute thread milling cutter equipped with a carbide insert. These inserts are expensive to purchase but allow us to operate at high cutting speeds unlike the majority of taps that are made from High Speed steel and must operate at low cutting speeds.
Once purchased, a 12 TPI insert or a 10 TPI insert can produce any diameter of thread with this number of threads per inch. Obviously unlike taps that must be purchased for each diameter and TPI style require.
Selecting a thread milling cutting
When selecting a thread milling cutter we should select the smallest diameter cutter available which will allow us to reach the bottom of the threaded hole. The smaller the cutter is, the higher the operating RPM for a given SFPM cutting speed.
Also consider the length to diameter ratio of the cutter to extend into the full depth of the hole. Again our judgment will be required to select the smallest diameter cutter for maximum RPM and productivity, against the potential of deflection caused by the cutter being extended excessively.
A limitation found in thread milling is a requirement for a deep thread.
This is when tapping will still be a good choice.
Problems with tapping: Size control
Recall that taps are supplied in different size specifications, H3, H5, etc. Many shops do not have a wide selection of taps on hand. When producing the correct size is required we may need to wait until the correct size tap is purchased.
As thread milling uses circular interpolation we can use cutter compensation (G41/G42) to control the size of the thread produced.
Join us here next month when we’ll discuss thread milling programming.
|
