FeatureCAM by Delcam
Salt Lake City, Utah
CAM software has come a long way since such packages required that an operator program every machining operation, and do so one at a time. To cut a hole, for example, programmers had to separately specify centering, drilling, reaming, tapping, countersinking, and counterboring. Users also manually picked speeds and feeds for each operation.
Recent feature-based software is altering that scenario, with more machining intelligence built into the program. Such software reduces programming time and provides more consistent NC code from part to part.
It's helpful to note that features are defined differently in CAD and CAM. Features in CAD can be additive or subtractive. For example, a CAD user might start with a block, remove a pocket, and add a boss or rib. Features in CAM, however, are always subtractive. So where a CAD designer deals with a pocket and a rib to divide one pocket into two, a CAM programmer thinks solely in terms of two pockets.
This can be important when files are imported from a variety of CAD systems into feature-based CAM packages. For example, FeatureCAM software pays attention to a few subtractive features such as holes in imported solid models, but it considers the model mostly as a collection of faces, deducing from the example above, for instance, that two pockets are required.
Features in the software can be thought of as building blocks to create a part. They are portions of geometry produced by a set of machining routines. Features define shape. Users select features such as holes, pockets, slots, step bores, and threads, and then type in their numeric dimensions. Or, users select features such as bosses, chamfers, grooves, and faces, creating them by chaining together curves and possibly entering additional dimensions. Features also describe how to produce the shapes on NC machines, and thus contain information such as a shop's preferred machining strategies for roughing and finishing.
The commonly used Hole feature is a good example of how programmers create a feature and associated machining operations. Selecting this option opens a dialog box into which users type hole dimensions such as length, width, depth, chamfer depth, and coordinate location. Programmers then assign a manufacturing process, such as first center drill, then drill, and lastly tap, and click a checkbox for chamfering.
Other operations come from default rules already programmed in the software. For example, a rule determines when pecking is to take place based on hole depth. Pecking pulls a drill out of an unfinished hole to break the chip and clear the hole of metal. The software includes thousands of such rules, each one fairly simple and with parameters users can easily tweak.
In general, programmers can type in settings based on a particular job, the material being cut, or even individual operator preferences. Users can specify shopwide rules such as when reaming a hole, always use a tool that is 98% the size of the finished-hole diameter. Or, they can apply a rule to only one hole.
After generating operations, the software selects the correct tools for each from its database of preloaded or user-defined cutting tools. The program also calculates feeds and speeds, which users can override as required, and then generates toolpaths and postprocessed NC code. When users make changes on features, the software updates associated end products.
AUTOMATING FEATURE RECOGNITION
Knowledgeable programmers generating NC using manufacturing features still have to provide information crucial to efficient part production. This process can be further automated by creating manufacturing features directly from imported solid or surface models. Users can use one of several methods to classify surfaces in the model as Feature-CAM manufacturing features.
When features are to be recognized by the software, a milling wizard creates them, for instance, by dividing the model into horizontal slices. The software recognizes features as side portions of the slices and generates plain, countersunk, and counterbored holes as well as rectangular pockets.
In a separate, less-automated technique, users import a model, click on the Feature button, and select several features. Only holes, slots, pockets, bosses, and sides can be recognized. Users click the Extract Feature button, pick Surfaces as the method, select the surfaces, and then confirm or modify dimensions and pick a machining strategy. A window displays the operations that will be used to manufacture the feature and identifies selected tools and calculated feeds and speeds. Or course, users can modify or accept these settings.
Another technique provides recognition of feature curves. For milled features that require curves such as bosses, pockets, and sides, the shape of features is determined by chaining the curves in the plane of the current user coordinate system. This technique works well for features that are made of too many surfaces to conveniently pick.
FeatureCAM by Delcam, featurecam.com