Single Point Broaching: C Axis Lathe Programming
Prior to broaching, bore a hole the size of the minor diameter of the finished form and approximately 75% deeper than the desired broaching depth. Next, create a chamfer going from the major diameter to the minor diameter of your form at a 45 degree angle. Finally, add a recess behind the bore diameter that is larger than the major diameter of the finished form to allow the chips to break after each pass.
Creating Your Main Broaching Program
Once the part preparation has been completed, the main broaching program must be created. In addition to the tool change info and initial cutting start point, the main broaching program should be created as a call program that contains the C axis rotation and subprogram information. The subprogram will control the incremental cuts that create each tooth or corner of the form you are trying to produce. The main program will control the C axis positioning and number of times the subprogram will be called. Set the number of times the C position will index based off of the number of teeth or corners to be created (ex. 8 teeth= 7 indexes following initial start position). Call the subprogram the required number of times between C axis indexes (8 teeth= 8 subprogram segments). The angle of the C axis rotation between subprogram segments will also coincide with the number of teeth/ number of corners of the final form. For example:
4 corners= 90 degrees
6 teeth= 60 degrees
8 teeth= 45 degrees
Creating Your Subprogram
As mentioned above, the subprogram will control the incremental cuts that create each tooth or corner of the form you are trying to produce. After feeding to the desired depth, you must program the machine to drop down then away from the tooth. This means that the subprogram will include the depth of cut in the X axis, distance of cut in the Z axis, the X retraction amount, Z retraction and number of loops.
Establishing your incremental Z value (distance of cut): Leave sufficient distance (1” recommended) in front of the workpiece to allow for acceleration before making contact with the part. Add that distance to the required distance of cut to get the value of your full depth. For example if the distance to be broached on your part is .650” and you are starting 1” in front of the part to allow for acceleration, the incremental Z distance would be 1.65”. Set the Z feed rate to rapid.
Establishing your incremental X value (depth of cut): Set your incremental X move in the positive at twice the depth of cut you require. In other words, whatever amount of material you want to remove per pass, double that value and add it to your retraction amount to get your positive X incremental value. For example, if you want a depth of cut of .001 and your incremental X retraction is -.020, your incremental X distance value would be .022.
Determining the required number of loops: The subprogram’s number of loops must coincide with the required tooth depth. For example, if the depth of cut (amount of material being removed per pass) is .001 and you are making a form with a tooth height of .090, the program will require 90 loops.
Using the above examples, the subprogram would be as follows:
IMPORTANT: These are general guidelines to be used as a reference point only. Each machine make and model will differ in how you should program. Know your machine and what it is capable of.