Holemaking. A layperson might think, “what could be simpler?” But a machinist knows better because there’s a lot to consider when creating a streamlined toolpath. Machine controls and programming software now support a range of complex capabilities, including multi-axis and high-speed machining, in-process monitoring and measurement, and lights-out operations. Software development now maximizes simplification and ease of use.
Programming a machining process typically involves defining parameters for each step of the operation. Producing a certain hole, for example, may require applying a spot drill, then a drill of the desired hole diameter, and finally a tapping cycle.
Recent software usability improvements include incremental upgrades such as one-click selection of all matching holes on a part. Software providers also offer automatic programming features that review part elements and list appropriate tools and parameters needed to complete a job. Such features are useful but require the user to separately validate each of the suggested toolpaths.
The goal is to easily create custom variations of existing toolpaths. For example, chamfering five holes of differing diameters would mean programming, typically, five separate toolpaths. The Chamfer Drill toolpath in Mastercam, for example, chamfers all of the holes with the same spot drill or chamfering tool. After choosing the tool, the user needs to define only how wide or deep the chamfer should be, and for each hole the software changes the depth the tool will run.
A more complex application further illustrates the benefits of simplified programming. Drilling a 7" (178-mm) deep, ¼" (6.35-mm) diameter hole requires a variety of tools, cutting parameters and tool motion commands. In this case, after a spot drill establishes the position of the hole, a short drill produces a 1" (25.4 mm) pilot hole. Then, the long, relatively delicate carbide drill that will complete the full hole depth feeds 0.5" (12.7 mm) into the workpiece at 150 rpm and a 10 ipm feed rate, with coolant turned off. Slow feed with no coolant pressure ensures self-centering and helps protect drill integrity.
The remaining hole depth is achieved at 1,280 rpm and 3 ipm feed, with flood coolant. Retraction at 200 ipm, with coolant turned off, follows a short dwell at the bottom of the hole to assure chip removal. Every step in the process, including feed rates, cutting depths, cutting speeds, coolant flow and dwell time can be listed on an Advanced Drill Cycle setup page in a fully customizable grid. Later, a user can return to the grid to customize the program for different but similar applications.
A particular challenge is drilling complicated workpieces that require custom cycles, such as aerospace honeycomb panels. These feature delicate aluminum honeycomb-like structures enclosed on both sides by a carbon fiber or aluminum shell. Piercing the shell requires a specific set of drilling parameters. Passing through the honeycomb requires other strategies, including even spindle reversal, to avoid seizing and tearing the honeycomb material. Exiting through the outer shell requires yet another approach. Advanced Drill Cycles permit detailed programming of each step, and users can revisit the program setup and adjust parameters as needed.
The intent is to make these kinds of programming capability and flexibility features available in entry-level, 2D software packages as well as in premium products. Smaller shops can benefit greatly from the increase in simplicity and time savings for practical automation strategies in machine control.
Connect With Us