Exploring Advanced Manufacturing Technologies. Steve Krar
for fatigue cracks.
MACHINING HINTS
In comparing HSM with conventional machining there are many different factors that must be considered to make the change to HSM cost effective. Some of the changes associated with HSM are cutting forces, cutting tools, speed rate, feed rate, toolpaths, and material removal. The following conditions may occur:
Fig. 2-1-25 Any tool fragment from a high-speed operation can be compared to a bullet. (Modern Machine Shop)
▪Cutting tool edge buildup – This can be a problem at high speeds for some combinations of cutting tools and materials.
▪Chip removal – Because of the large volume of chips created, they must be removed quickly form the machining area. Horizontal machining centers (HMC), where the chip falls away from the machining area, seem to resolve this issue.
▪Rigidity – Higher speeds can produce some unwanted vibration that may require a sturdier machine to overcome.
▪Cutting tools – Longer-life tools, such as coated, CBN, or diamond, are required to avoid the time lost due to frequent tool changes.
CNC
In high-speed milling, the control system electronics can make all the difference, Fig. 2-1-26. The right CNC, together with other elements of the control system, can let a slower machine tool mill a given form faster than a machine with a higher top feed rate. The reason is that in any milling routine that is relatively complex, the control system determines how much of the available feed rate can be put to use.
Overall System
A control system is only as fast as its slowest component. Improvements in CNC control systems have made HSM possible and the limiting factor seems to lie within the machine tool itself. Technologies related to HSM touch on every link in the CNC loop.
Fast Processing
Fast CNC processing speed is fundamental to HSM. This is particularly true where the CAM software has defined a complex tool path as a series of numerous short moves. If the CNC cannot process these blocks faster than the machine can move through them, then the machine will stutter as it waits for data. Slow data input to older CNCs can produce a similar effect.
Fig. 2-1-26 The control system of a CNC machine plays an important role in high-speed machining. (Modern Machine Shop)
Input Baud Rate
With an older CNC machine, input baud rate is the bottleneck that can severely limit feed rate. When a program must be drip fed through a serial port, the CNC can’t execute the program commands any faster than it can receive them across this connection, Fig. 2-1-27.
Newer CNCs overcome this bottleneck in either of two ways. They provide enough memory for a long program to be stored at the control so that drip feeding is no longer necessary. This also allows for network connections (like Ethernet) that permit much faster program transfer than the serial link.
Machining Rate
The need to drip feed across a serial connection can impose a feed rate limit for effective machining. The maximum feed rate is a function of the serial connection’s baud rate.
Assume each character commands 10 bits of data. A serial connection with a baud rate of 38,400 bits per second can therefore transfer 3,840 characters per second.
Factors including the memory required for DNC overhead will limit the maximum effective feed rate to a value somewhat lower than this.
▪On older CNCs, a common serial baud rate is 9,600. At this rate, the maximum feed rate drops to below 60 in/min. Therefore it may not be possible to perform effective high speed milling of complex regions of the part where such a slow drip feed is required.
Fig. 2-1-27 A slow baud rate can severely limit the feed rate. (Modern Machine Shop)
LOOK AHEAD
In complex milling, the tool path segments can be so short that a machining center moving at a high feed rate cannot speed up or slow down fast enough to make direction changes accurately. Corners may be rounded off and the workpiece surface may be gouged, Fig. 2-1-28. The Look-Ahead feature of high performance controls allows the CNC to read ahead a certain number of blocks in the program and when sudden direction changes are required, it slows the feed rate accordingly.
Number of Blocks
How many blocks a look-ahead feature looks ahead will vary from control to control, and more blocks do not necessarily mean better performance. A stiffer, more responsive machine can follow a tool path accurately with less advance warning from the control.
NURBS INTERPOLATION
Some CNCs can interpolate axes along mathematical curves. Asingle program block can describe a complete curve that might once have required several blocks of short lines to describe. When the CNC has plenty of processing power, curve interpolation lets the control system change direction along the curve more gradually, maintaining a higher average feed rate than it can when cornering from one straight line segment to the next.
NURBS (Non-Uniform Rational B-Spline) Interpolation is one type of curve interpolation. To take advantage of the capability, one requirement is a CAM system capable of outputting NURBS tool paths.
DIGITAL DRIVES
Machining centers for HSM generally use digital servo drives to maintain accuracy at high feed rates. The alternative, analog drives, may include lag time on the order of 10 milliseconds. A machine moving at 90 in/min. will move .015 in. in that time. Digital drives execute motion commands within a tighter margin, making it possible to combine high feed rates with high precision.
Fig. 2-1-28 The Look-Ahead feature of high performance controls allows the CNC to read ahead a number of program blocks. (Kelmar Associates)
High Resolution Feedback
Another advantage of improved processing power in the CNC system is the ability to use higher resolution feedback to monitor and control axis positions. This is particularly useful where the goal of HSM is to produce a smooth finish with little need for subsequent polishing.
PROGRAMMING
High-speed machining makes the tool path a more significant factor in the process, Fig. 2-1-29. Taking lighter cuts with a smaller step-over increment is only one consideration. An effective tool path also protects the tool by keeping cutting load steady and keeps a high feed rate by avoiding sharp changes in direction.
Programming a smaller depth of cut for roughing with a faster feed rate using positive rake cutters will assist the machining process. Finishing is recommended using Z-level machining (climb cut, pick over, and conventional cut) to produce better surface finishes.
Decisions made during programming can also affect the quality of the workpiece. If the purpose of HSM is to machine a smooth surface, the tool path may contribute to this goal.
Fig. 2-1-29 The tool paths created for machining a part. (FeatureCAM/Engineering Geometry Systems)
HIGH FEED RATES
A