|Expert Machinist, a knowledge-based feature, supports associative, parametric, and feature-based machining for 2.5-axis milling, and machining of prismatic parts common in production machining. The feature stores and reuses preferred machining methods. |
|Five-axis machining in Pro/NC Wildfire keeps the tool's leading edge on the material being machined. Routines that look for gouges and collisions include the tool and its holder. |
Pro/NC Wildfire generates toolpaths for all NC applications and includes a tool library, material database, process modeler, cutting simulators, and an API for customization. Users can machine directly on Pro/E data and other files from the developer's software, such as Cadds CVNC and Pro/Desktop. The NC software also accepts Catia files and formats from IGES, STEP, DXF/DWG, ACIS and Parasolid translated files. Users store and reuse manufacturing strategies along with parameters for a specific toolpath.
The milling module supports volume, thread, and plunge milling, roughing, reroughing, surface machining, engraving, pencil tracing, and hole making. Roughing operations include roughing only, roughing and cleanup, and profile only. Cutting strategies include one-way only, zigzag with different types of connections, and spiral inside-out and outside-in. Approaches to material includes entry through approach walls, ramp angle, helical plunge, plunge in predrilled holes, and by plunge in previously machined areas. For multicavity roughing, cutting is by region or slices, which is appropriate for thin-wall machining. PTC is one of the few that supports plunge roughing, which is useful for removing large amounts of material from deep cavities. It usually reduces cycle time, improves heat dissipation, and puts a uniform load on the cutting tool. In reroughing, the NC software creates toolpaths to machined areas not reached by previous roughing sequences.
Pockets, a common milling task, are cut level-by-level or pocket-by-pocket. Level-by-level pocketing is for machining thin-walled objects. The NC software handles an unlimited number of pockets and islands. Pro/NC sorts and machines nested pockets in a single operation. It also produces open and overlapping pockets.
IGES models are, of course, not feature based. Users must define features on them, such as holes, slots, and pockets, and then apply machining processes to them.
In-process models are used when partly machined parts move from one machine tool to another. Although the software knows the depth of material remaining on in-process models, for some reason it's not shown in 3D simulations. Oddly, 2.5-axis turning operations does show such changes.
Holes are made with custom cycles or with a feature called Autodrill. Many cycle types are available in standard Pro/NC. Users select holes by diameter, surface, axis, drill groups, or by points. Autodrill lets users create, store, and reuse a library of hole-making strategies.
Basic lathe operations in the software include roughing, facing, grooving, threading, and finishing. More advanced turning operations include synchronous or balanced turning for four-axis lathes, support for lathes with multiple turrets and subspindles, a mill-turn capability, and support for Swiss-turn machines.
Turning toolpaths are optimized for production and prototype work. An option lets users work in 2D or 3D. The 3D environment includes reference parts, stock, fixtures, and tooling. The software also generates viewable in-process models.
The software synchronizes two turrets cutting the same part on a single spindle. Users also pick areas that need synchronization. Visualization shows virtual turrets following these toolpaths. In Pro/NC, two toolpaths are generated in a single program and postprocessors support the operations.
Mill-turn machines, also supported, mount a milling head on a turret to allow facing, producing slots, and cutting holes into turned parts. Pro/NC performs this as one operation to generate synchronous milling and turning operations in a single program.
Several of the milling and turning operations include five-axis milling. Subspindles are supported, but the software doesn't simulate parts transferring from one spindle to another. Mill-turn operations can run simultaneously, sequentially, or in a combination.
PTC is one of the few vendors to support Swiss-turn machine tools. These machines are specialized lathes with continually fed bar stock.
The software includes a library of cutting tools, tool holders, and fixtures. Cutting tools are referenced by parameters or by solid tools for simulation. Optimum feed, speed, and depth-of-cut are stored for each cutting tool and are a function of material and application. Users can query external tool-data-management systems and load the tool into the Pro/NC tool database. However, tool creation and management need further improvement.
Batch processing generates toolpaths off-line. This is helpful when generating complex and long toolpaths, such as those commonly found in dies. If the processor supporting Pro/E is networked, files can be sent to a server for background processing.
The software also generates process documentation, such as assembly process plans, setup sheets, tool lists, and information for fixture and jig designs. The data is in HTML for Web access.
Three to five-axis contour milling is done on solid models or directly on surface models. The software sports several three-axis finishing strategies including parallel-plane machining for parts with relatively flat surfaces, Z-level finishing for parts with steep surfaces, and flat-surface machining in which the software locates flat areas and then machines them. There are about eight other approaches. Unfortunately, the program does not support 3D or equidistant stepover options, a method that produces particularly smooth surface finishes. It is common in three-axis milling.
The software's rest milling exploits the fact it knows the previous tool used and the selected one. Rest milling generates toolpaths to remove only the material left behind in valleys, depression, ridges, or corners. It can remove material left by a previous volume, profile, surface, and local milling operation.
High-speed machining is essential in mold and die operations. The tactic here finds a toolpath that maintains constant cutting conditions and a constant chip load on the tool during machining. The constant chip load produces a constant rate of material removal and eliminates load spikes. This allows a more aggressive machining strategy and lets machines run at optimal speeds. It also minimizes accelerations and deacceleration.
Three-plus-two machining, also called five-axis positioning, is often used for milling deep cavities. It includes profiling, conventional parallel-plane milling, and isoline milling that follows the U-V curves or user defined flowlines.
Each Pro/E Wildfire license includes one for CG Technology's Vericut, a material-removal simulator, and a license for Intercim Gpost for postprocessing to specific machine tools. Pro/NC produces ASCII APT-based CL-files that follow ISO and ANSI standards, so it's supported by all standard postprocessors.During simulation, Vericut displays gouges, tool crashes, and undercuts. Collision detection includes cutting tools, toolholders, and fixtures.
To drive CMM machines, PTC generates code in DMIS 3.0, a format read by most measuring machines. However, the developer does not provide a CMM postprocessor, so it is difficult to modify output formats or data. Pro/NC Wildfire comes from PTC Inc., 140 Kendrick St., Needham, MA 02494, (781) 370-5000, www.ptc.com
-- Alan Christman
Alan Christman is vice president of CIMdata and resides in Boca Rotan, Fla.