Automatic Drill Toolpaths

The Automatic Drill toolpath create a complete series of drill operations for a set of arcs or points. For example, after selecting a set of holes, Mastercam can automatically create a sequence of spot drilling, pre-drilling, tapping, and chamfering operations.

NOTE

When working with solid models, use FBM Drill to detect holes in the solid based on specified criteria, and automatically generate a complete series of drill operations for selected features.

Mastercam automatically selects drills from the tool library that you specify and matches them to the diameter of the selected arcs for each drilling cycle that it creates.

If you select points, Mastercam prompts you to specify the final diameter of the hole to drill at point locations. You can mix arcs of different diameters and Mastercam automatically selects the proper drills. However, you can only specify a single hole size to be used for the points; so if you want to drill holes of several different diameters, you should create arcs in your part. Mastercam does not drill a hole if it cannot find a matching drill in the tool library.

The drill cycles used in each operation are determined by the cycle stored with each tool definition. (If you select a flat end mill as the finish tool type, Mastercam uses a drill/counterbore drill cycle for the finish drill cycle.) Mastercam only uses cycles that have been enabled in the active control definition on the Machine Cycles page.

The result of the automatic drilling process is a series of individual drill operations that are listed in the Toolpaths Manager. You can then review, modify, move, or regroup each operation individually without affecting the others, using any Toolpaths Manager function. The operations are not associative with each other after Mastercam generates them; in other words, if you change one operation after it has been generated, Mastercam does not automatically change others in response. You cannot go back and directly edit the auto drilling parameters. Consider using the Edit Common Parameters dialog box if you need to change values for toolpath settings that affect all or several of the operations.

To begin using the automatic drilling function, follow this general outline:

  1. Select Auto Drill from the Mill or Router contextual tab.
  2. The Toolpath Hole Definition function panel displays so that you can select the drilling locations. Once you have finished, click OK.

    NOTE

    To select arcs, choose Mask on Arc, and then select an arc of the desired diameter, or choose Entities and use the Selection Bar options to select the desired arcs.

  3. The Tool parameters tab displays so that you can begin to enter the drilling parameters. Click the help for each tab to learn more about filling in the parameters to create the drilling operations.

Learn more