A HIGH-PERFORMANCE TOOLPATH TO FIVE-AXIS MACHINING
To fully gain a competitive edge through five-axis capabilities, a shop must first decide what milling techniques, toolpaths, and coinciding cutting tools to use for these machining operations. This primer can help make those decisions.
The benefits of five-axis machining are numerous. With it, shops can efficiently and accurately machine complex 3D component features to superior surface finish quality, minimize part setups, reduce secondary machining operations, incorporate shorter tooling to avoid collisions, and boost metal removal rates. The list could go on, but none of these benefits will come to fruition until shops first decide on what milling techniques, toolpaths, and coinciding cutting tools to use for their five-axis machining operations.
Milling technique, toolpath, and cutting tool selection are key factors for successful five-axis machining. Two milling techniques are point milling and flank milling, which encompass the use of high-performance toolpaths that will optimize five-axis milling.
The portion of the cutting tool that will be doing the cutting differentiates the two milling techniques, which determine toolpath and cutter type. Each technique involves high-performance toolpath approaches that are incorporated at the CAD/CAM stage of part setup.
Flank milling is, as the name implies, milling where the side of the cutter performs the machining and the tool’s radius, if included, generates only the component fillet radius. Flank milling provides shorter cutting times than point milling, but can be limiting in some respects. It is most suitable for semi-finishing and finishing operations, but only on single-curved and convex surfaces. The larger the tool or greater the amount of cutter engagement, the more power, torque, stability, chip evacuation and machine movement capability are required.
When flank milling in five axes, cutting tools should have adequately long radial cutting edges, such as on solid carbide endmills or exchangeable head cutters. These can be either straight or conical and have various corner radii.
There are several high-performance toolpath techniques for flank milling, including trochoidal, slicing, and profiling. For these, small blend radii are required, and conical ball-nose endmills deliver the added advantage of stability, as compared with standard ball-nose endmills.
Trochoidal milling is a roughing technique that uses three machine-axis movements. The tool follows along a continuous spiraling toolpath, feeding in a radial direction in confined spaces to remove large amounts of material. The tool continually advances forward for each cut, generating a groove or profile pattern. Large depths of cut using relatively light cutting forces are possible with trochoidal milling because radial depths of cut involved with the process are quite shallow.
Slicing, or machine movement in three axes, is a semi-roughing/finishing technique for component corners that usually requires high speed and dynamic machine capability. This type of machining involves toolpaths of many passes taking minuscule radial depths of cut so that large axial depths of cut can be taken in high corners.
During profiling operations, toolpaths maneuver cutting tools so that only their flanks are cutting, a process for 2D machining. For 3D machining, the cutting tool’s flank is cutting as its radius simultaneously cuts the bottom part surface. As with slicing, profiling also requires high-speed dynamic machine capabilities and stability to be effective.
For point milling, which is done with the ends of cutting tools, shops can choose from a number of applicable cutting tool types, depending upon the component features and finish requirements. Generally, for larger, open surfaces, toroid or bull-nose type milling cutters are preferable. For cavities, ball nose cutters are often the best choice. Conical tools can be used for long overhangs, as well as modular tooling with reduction adapters that provide maximum stability when extended tool reach is necessary.
Bigger diameter tools can be used for roughing operations, but doing so depends on machine tool capability and surface requirements. In semi-finishing operations, the toolpath strategy should be to mimic the finishing operation toolpath. This will garner the best results when five-axis machining. Also, the aim should be to leave the same amounts of rest material over the entire workpiece surface for the finishing operation.
For finishing operations, tool selection is dependent upon the surface finish and level of part accuracy needed. While several different types of cutters can optimize simultaneous five-axis machining, toroid cutters can be used on a more general basis and ball nose cutters applied in the case of more demanding cuts, as with closed pockets.
LEAD AND TILT ANGLES IN THE CAD/CAM PROCEDURE
The way a rotating cutter is presented to a component surface is a primary consideration for optimized five-axis machining. For this reason, lead and tilt angles are a critical part of the CAD/CAM toolpath-generating procedure and should be established during the set up process. Not only should the entering angle of the cutting edges be determined, but also cutter engagement and clearance, so as to avoid back-cutting.
Lead angles are measured between the centerline of the tool and the perpendicular plane of the workpiece surface at the point of tool contact and in the direction of intended feed. In many cases, the determined lead angle is kept constant according to recommendations for the tool to be used, but can be varied through programming if the CAM system is capable.
Through a locked lead angle, the cutter is inclined at a pre-determined angle throughout the feed direction in relation to the component surface. The lead angle is established at the smallest internal radius on the surface and the effective diameter of the cutter.
The tilt angle of a cutter is established within the plane that is perpendicular to the direction of feed and, therefore, to the lead angle. A constant lead angle in the point of cut is necessary for generating curved and concave component surfaces, and although point milling consumes more cutting time and tool life, it is a safe method to use for concave and double-curved surfaces.
Additionally, 3D surfaces are generated by successive levels of cutter passes where the tool is engaged with the workpiece at a point on its corner radius. This point will vary along the radius according to the surface. Point milling with an endmill can be applied to roughing, semi-finishing, and finishing operations.
Part surface finish is a matter of tool stepover in relation to cutter diameter. This relationship also directly affects machining times.
With toroid cutters, cutting times can be reduced considerably in relation to a ball nose cutters used for conventional copy milling. When developing toolpaths, shops must keep in mind that the relationship between stepover and diameter has a maximum of 1 to 2 for toroid cutters, where large stepovers reduce machining time but leave higher degrees of surface roughness.
In this context, the ball nose cutter does not provide the same productivity and favorable machining conditions. The cutter will form a surface with a certain cusp height depending upon the combination of feed per tooth and width of cut. The depth of cut will influence cutting forces and levels of tool stability required. With this said, achieving a smooth, symmetrical surface finish is a function of cutter tilt, feed value, direction of cut and tool holding, all of which should be optimized to achieve the proper balance.