G32 - Threading with Control

     In this space we've talked about using G76, a canned cycle threading command that is easy to program. Another popular threading command is G32.

     The G32/G33 method is the traditional thread programming command. It is often output from CAD/CAM software packages when you ask for a threading routine. Although CAD/CAM software makes programming easier, it is always helpful to understand the codes and exactly what they mean. Let's take a look at the G32 threading program.

     The two biggest advantages to the G32 method are that you, as the writer, can control the depth of each thread pass and the exact plunge angle.

     To cut a thread, the tool makes many passes, taking shallow cuts down the angle of the plunge.

     In our example, we'll program a 4" diameter, 12-pitch thread, 2" long. As the programmer, you must determine the X and Z positions for each pass.

     The first step is to determine the plunge angle at which the insert approaches the part. We are using a 29˚ angle in our example. Next, at what Z position will the tool start to make the first pass? To allow for the acceleration of the Z axis slide, we normally start the routine approximately 4 pitches from the beginning of the thread feature. We are programming a 12-pitch thread, so we have started at the Z0.400 position.

     Tooling manufacturer supply recommendations for the depth of each pass. This information is generally found in the tooling catalogs. The tooling catalogs reveal that the depth of each pass gets smaller as you approach the final thread depth (the minor diameter).

     As the tool gets deeper into the thread, the area of contact between the part and the tool increases. Taking more shallow cuts allows for this increase in contact and reduces the chance for work hardening.

     Now, we know the Z start point for the first thread pass and the X dimension for each pass (depth of each cut), but we do not know the Z position for each pass.

     A simple trig calculation provides this value.



     The triangle shown here is found by using the depth of a threading pass and the 29˚ angle and then using the tangent function to calculate the Z distance for that pass.

     TAN 29˚ x depth of pass = Z distance

     Here is the sample program showing several threading passes.

     Calculate the difference between the X diameters block N110 and N150 (3.9812 - 3.9461) ÷ 2 = 0.0085. Multiply this radius value by the tangent of 29˚ (0.0085 x TAN 29 = 0.0047). This is the incremental distance in Z between block N100 and N140 (0.400 - 0.0047 = 0.3953). Now use this method to check the Z value in line N180.

     By using G32 you can control the exact depth and distance of each machining pass. Even if a CAD/CAM system provides the code, with a few simple calculations you can better understand the program and the machining process.