When 2+3 Doesnt Equal 5

Dec. 21, 2007
Fewer moves deliver precision from five-axis machines.
Makino’s 5-axis machining center.

Many shops realize that five-axis machining is a quick way to machine multiple part sides in one clamping to reduce setup times and shorten lead times. But what they may not know is that full, simultaneous five-axis machining is not always the most accurate way to cut parts. Instead, five-axis positioning, or what is known as 2+3 machining, can add up to more precise machining operations.

While all a machine’s axes move simultaneously for full five-axis cutting, only three axes -– X,Y, and Z -– move for 2+3 machining. The other two rotary, or secondary, axes are used only for positioning. Once a part is oriented to allow the use of standard three-axis machining movements, the secondary axes are locked in place and do not move during the cut. A good 2+3 machining example is cutting an angled surface after it has been positioned as a flat surface.

Bill Howard, VMC product manager for Makino (, said a five-axis machine’s secondary axes are inherently less accurate, while its three main axes are more precise for positioning and repeatability. That is the reason that he believes 2+3 machining lets shops, especially those doing die/mold work, take full advantage of the precision built into a five-axis machine tool.

“It is the highest potential for precision because the two least accurate axes are positioned and locked in place, while the machine’s three other, more accurate axes do the machining,” Howard said. Other benefits of 2+3 machining include optimized tool contact with machined surfaces, minimized setups, increased quality, and faster throughput.

2+3 machining positions workpieces for making standard 3-axis cuts (top), while in full 5-axis cutting (bottom), cutters work their way down the angled surface.

With 2+3 machining, shops can maneuver cutting tools for optimum cutting engagement and use short, stiff, rigid high-speed tooling. Such tooling lets them run at higher rpm and at more-aggressive feedrates for smaller, finer increments of surface milling. Optimized tool contact also maximizes tool life.

Especially for die/mold work, 2+3 machining reduces part setups by providing access to multiple sides of parts, including cores and cavities, with one clamping.

Fewer setups and less part handling reduce the risk of stacked tolerances and make for tighter tolerances between all surfaces that are milled in a single setup. All of these benefits combine to improve part quality and surface finishes, and to reduce benchworking.

Because 2+3 machining is quicker to program than full five-axis machining, the technique also increases throughput. And while most conventional programming systems support full fiveaxis programming, almost all of them support the 2+3 approach.

In addition, full five-axis program toolpaths are longer and lead to extended cycle times, and optimizations or changes are more difficult to support in a full five-axis mode, Howard said.

Controlling five axes
Shops that are considering going from three-axis machining to five-axis, simultaneous machining should look for specific features in a machine’s control system to simplify the transition. These features also can help to get the best performance possible out of CAM-generated data to improve the entire machining process.

Gerry Traicoff, manager of technology transfer at Hurco Companies Inc. (, said three helpful control features or functions for full, simultaneous fiveaxis machining are: tool centerpoint management, linearization and the ability to specify a tool vector instead of specific axes of rotation. And, for shops that are moving into five-sided machining, Traicoff advised that they should consider a control with some type of positioning function to reduce the number of part setups.

Tool centerpoint management functions help to simplify several tasks, including programming, tool set up, and posting part programs to machines. This control function posts programs so that all tool motions are relative to part zero. So, at the CAM stage, parts do not have to be transformed based on where a workpiece is fixtured on the machine tool.

“Part setup is independent of where the workpiece stock is fixtured on the machine,” Traicoff said.

Shops without tool centerpoint management in the machine control have to fixture stock on a machine, then calculate the distance from part zero to the center line of machine rotation. Once that distance is known, the CAM programmer applies a transformation before posting the toolpath on the part. The machinist at the machine then touches off all the tools at part zero.

However, if the machinist shifts the stock on the machine, the programmer must have those new coordinates to apply a transformation again.

With tool centerpoint management in the control, CAM programmers simply program to part zero and do not have to worry about the zero centerlines for machine rotation. Transformation takes place at the machine tool, where tooling and part zero both are calibrated at the centerpoints of rotation.

“When linearizing rotary axes for full five-axis machining, errors can arise due to tolerances when posting out programs,” Traicoff said. If linearization is built into a machine’s control, shops can add a higher degree of interpolation to smooth a machine’s rotary-axis movements and to create shorter toolpath programs.

Hurco’s VMX 42SR includes control functions that ease 5-axis machining.

The capability to specify a tool vector instead of specific axes of rotation for full five-axis machining lets shops post out tool vectors from their CAM systems to their machine controls. They can program the center of the bottom of a cutting tool as X, Y, and Z then the vector, or orientation, of the tool as I, J, and K. There are no rotary address Hurco’s VMX 42SR includes control functions that ease 5-axis machining. commands -– no A, B or C. Shops simply command the machine to move the tool tip in a specified orientation vector.

The key advantage of this control function is that a part program can run on any five-axis machine tool without having to repost the program. This is especially useful for shops that run multiple five-axis machines.

Latest from Machining / Cutting