Читать книгу Exploring Advanced Manufacturing Technologies - Steve Krar - Страница 16
Оглавление(Steve Krar, Consultant—Kelmar Associates)
High-speed machining (HSM), in order to be most effective, must involve the correct selection of machine tools and controls, cutting tools, and programming. HSM uses high spindle speeds, high feed rates, and light depths of cut to increase productivity, reduce lead time, reduce warping, increase part accuracy, and improve surface quality. High-speed machining begins at 12,000 surface feet per minute (sf/min.) and may be as high as 18,000 sf/min and feed rates of 600 in/min. when machining aluminum. This requires a machine that can produce a spindle speed of 8,000 revolutions per minute (r/min) or higher.
The speed in High Speed Machining (HSM) is the speed at which CNC machining can replace the operations of polishing, assembly, unused shop capacity, and other manufacturing delays. Run fast enough, and machining centers become an economical alternative to more dedicated systems for a variety of production parts. If after careful evaluation, the cycle time of each operation can be reduced even by a small amount, it could produce big savings in production time and cost.
The goal of High-Speed Machining should not only focus on the speed of machining but also the flexibility it provides. Batch jobs can be run with little advance notice, streamlining inventories, Fig. 2-1-1. The speed can let CNC machining centers compete effectively for parts that would once have required a more dedicated manufacturing process. The key factors that affect the efficiency of a HSM system are the machine tool, the controller, spindle, toolholder, cutting tool, and programming.
Fig. 2-1-1 High-speed machining focuses on speed and flexibility. (Cincinnati Machine, a UNOVA Co.)
MACHINING CENTERS
HSM allows CNC machining centers to compete with a dedicated manufacturing system such as a transfer line. The machining centers can deliver these benefits:
▪The reduction or elimination of non-cutting time by minimizing tool-change time
▪Produces more parts than machining with a slower spindle and deeper cuts
▪Better surface finish that can eliminate operations of grinding and hand finishing
▪Minimal warping of monolithic (large) parts such as those common in the aerospace industry
▪The production of single complex parts that replaced sections formerly made up of a number of parts
▪Freedom to change part number – To set up a dedicated system because of a design change might require months of downtime while machining centers can be updated in a matter of days.
▪Fast response to engineering changes - Any machining center can be equipped to run multiple part numbers, giving the manufacturer flexibility to respond to customer needs.
Fig. 2-1-2 High-feed rate contouring requires high responsive ways and drive motors. (Modern Machine Shop)
Complex, high-feed-rate contouring requires high response from the ways and drive motors of the machine, Fig. 2-1-2. HSM may also affect the choice of machine hardware. How well the machine manages heat may be a factor. And the freedom to take lighter cuts might permit a different method of contouring.
MACHINE TOOL WAY SYSTEMS
The way system is the part of the machine tool that holds linear motion on track in each axis. There are two basic types:
1.Box or hardened ground ways usually found on conventional machines consist of a box-shaped stationary way that mates with a slide. A thin film of oil is pumped between them to keep the slide moving, Fig. 2-1-3A.
2.Linear guides found on newer machining centers have a linear bearing system that rolls along a guide way. This guide way is usually shaped in a way that helps the bearing grip it, Fig. 2-1-3B. Most machining centers designed for HSM use linear guides.
Fig. 2-1-3A Conventional machine tools are usually equipped with box ways. (Fadal Machining Centers)
Linear Guide Advantages and Disadvantages
Linear guides are a low-friction way system that reduces axis reversal error. Compared to box way systems, linear guide systems have a shorter life since linear bearings have moving parts that wear out. Linear guides provide less damping than box ways. Additional damping in the machine structure can make up for this. The linear bearing design can also influence vibration.
▪Virtual Ways
The advanced state of control technology allows some machining centers to use interpolation only - no way-system hardware, to achieve linear motion in X, Y and Z axes.
▪Thermal Stability
Single-setup machining and dry machining can both lead to large variations in machine temperature. Machine features for minimizing thermal distortion may become important. Some machining centers circulate coolant through the spindle and/or ball screws.
LINEAR MOTORS
A linear motor, an alternative to the rotary motor, can be thought of as a rotary motor unrolled flat, Fig. 2-1-4. It does not require ball screws to move machine slides. The lack of a ball screw makes the linear motor stiffer. On conventional machines, the ball screw and drive train are sources of backlash.
The linear motor has been applied to some CNC machine tools and offers high feed and high acceleration rates.
Advantages
▪Less vibration, less wear; a linear motor transmits force through a magnetic field instead of mechanical linkage.
▪Requires no contact between moving parts, except in the way system. Reduced contact between moving surfaces translates to reduced wear and reduced vibration.
Fig. 2-1-3B Linear guides are found on newer machining centers. (Fadal Machining Centers)
Fig. 2-1-4 A linear motor is a rotary motor unrolled flat. (Ingersoll Milling Machine Co.)
▪High accuracy at high feed rates lets the machine position, interpolate, and contour more accurately.
▪Faster machining for large workpieces since the linear motor is unaffected by its length of travel.
HIGHER CUTTING SPEED
On many machining centers, the metal-removal process is the key to HSM. Only higher speeds and corresponding feed rates during the actual machining process can produce improved time reductions, Fig. 2-1-5. Functions such as rapid traverse and tool change time are fast enough and therefore they do not have a great effect on the metal-removal process.
SPINDLES
A high-speed spindle is the most important part of the high-speed machining process, Fig. 2-1-6. In order for high-speed spindles to operate effectively, they require higher performance slide/servo requirements of the machine tool. The CNC control, cutting tool, machining center, and other components must be designed with the goal of using the higher spindle speed productivity. A conventional machining center can be retrofitted with a faster spindle, better cutting tools, and programming changes to produce some of the benefits of HSM.
Fig. 2-1-5 Higher speed and feed rates can reduce cycle times. (The Association for Manufacturing Technology)
Fig. 2-1-6 The high-speed spindle is the main component of a high-speed system. (Modern Machine Shop)
Spindle Compromise
A high-speed spindle presents a tradeoff between cutting force and cutting speed.
▪High-speed spindles generally have direct-drive motors, meaning the motor must fit inside the spindle housing and therefore their size is limited.
▪A limiting factor in high-speed spindles is the bearing that trades stiffness for speed. This is why most high-speed machining generally use light depths of cut.
Types of Spindle Bearings
▪Hybrid Ball Bearings - Composite ceramic bearings take the place of all-steel ball bearings in most high-speed spindles, Fig. 2-1-7.
•In a hybrid ball bearing, the race is still steel but the balls are long-life ceramic balls that deliver more stability at high speeds.
•The balls are lighter and stiffer, so they deflect less from centrifugal force, improving efficiency and reducing vibrations and stresses.
Fig. 2-1-7 Ceramic bearings are in most high-speed bearings. (Fadal Machining Centers)
Fig. 2-1-8 In hydrostatic bearings there is no contact between moving parts. (Fisher Bearing)
▪Hydrostatic Bearings - Higher-power high speed spindles, and spindles with high DN number, are equipped with hydrostatic bearings where there is no contact between moving parts, Fig. 2-1-8. Instead of steel or ceramic balls, a fluid, most likely water, supports the spinning shaft. Their advantages are stiffness, low runout because the fluid pressure tends to hold the shaft on centerline, and low maintenance.
OTHER NON-CONTACT BEARINGS
Air Bearings
An air bearing spindle’s superior runout characteristics that combines low runout with high speeds make it possible to machine effectively with delicate tools. An air bearing is a low stiffness bearing best suited for the lightest cuts. Where high-speed drilling generally implies light cuts taken quickly, effective milling with an air bearing is limited to very light cuts.
Magnetic Bearings
The spindle shaft is supported by a dynamic magnetic field and its stiffness can be digitally controlled to offer stiffness comparable to that of a ball bearing, Fig. 2-1-9. Magnetic bearings do not require a separate system to deliver air or hydraulic fluid.
Fig. 2-1-9 The spindle shaft of a dynamic magnetic field that serves as a bearing. (IBAG)
RETROFIT SPINDLE
Gain some of the advantages of high-speed machining by retrofitting a high-speed spindle to an existing machining center, Fig. 2-1-10. There are various types of retrofit spindles available such as replacement, fixed centerline, and secondary. Each spindle has options that are unique to them.
Fig. 2-1-10 Retrofit high-speed spindle options. (Modern Machine Shop)
Replacement Spindle - The machine’s existing spindle is replaced with a high-speed spindle. This option gives the retrofit spindle access to the machine’s entire work zone. However the machining center may lose the capability it once had to perform slow, deep cutting.
Fixed Centerline Spindle - An independently powered spindle that is mounted in the original spindle. The high-speed spindle can be removed to let the original spindle take slower, heavier cuts.
Fixed Centerline Options
Air powered spindle - If HSM is limited to very light milling and drilling with small tools, particularly in softer materials, then a spindle powered by air may be sufficient.
Spindle speed increaser - This device can increase spindle speed at the cost of some lost Z-axis travel. The increaser, shown in Fig. 2-1-11, uses planetary roller bearings in place of gears. An 8X version of this increaser delivers speeds up to 50,000 r/min.
Secondary Spindle - An independent high-speed spindle that is attached alongside the main spindle, Fig. 2-1-12. This leaves the original spindle available for slower, heavier cuts.
▪The secondary spindle is not centered along the X axis. On a typical vertical machining center, this causes the secondary spindle to lose access of 30-40% of the work zone in the X direction.
Fig. 2-1-11 A spindle speed increaser can deliver speeds up to 50,000 r/min. (Koyo Machinery)
TOOLHOLDERS
In toolholding systems consisting of spindle, toolholder, and cutting tool, the toolholder is the most important link because it has the greatest effect on the overall concentricity and balance, Fig. 2-12-13. As spindle speed increases, the choice of toolholder has the greatest effect on the effectiveness of the machining process.
Two-Face Contact and HSK
Centrifugal force from fast spindle speeds can cause the toolholder to retract when the spindle and holder touch only along the taper. The HSK toolholder that provides two-face contact at the spindle interface can solve this problem. Fig. 2-1-14. Two-face toolholder contact is worth considering for any machining center run at 12,000 r/min. or faster.
Two-Face With Conical Taper
Standard toolholders leave a space between the flange and spindle nose. Some toolholder systems close this gap to achieve two-face contact with a conventional taper, Fig. 2-1-15A and B. Both systems use toolholders with a special or modified spindle interface. Both designs permit the use of regular toolholders when two-face contact isn’t required.
Fig. 2-1-12 An independent high-speed spindle attached alongside the main spindle. (Precise Corp.)
Fig. 2-1-13 The toolholder is the link that has the most effect on concentricity and balance. (Command Tooling, Inc.)
Fig. 2-1-14 Two-face contact prevents the toolholder from retracting due to centrifugal force. (Modern Machine Shop)
CONCENTRICITY & BALANCE
Concentricity and balance are very important in high-speed machining, Fig. 2-1-16. Concentricity measures how closely the toolholder aligns the tool to the centerline of the spindle. A concentric grip helps ensure that all cutting edges will take the same depth of cut. Balance measures the distribution of weight of the tool and toolholder together. A balanced toolholder is critical for producing high-quality surface finishes, extending spindle life, and reducing or eliminating vibration that can affect the metal-removal process. A perfectly balanced tool and toolholder combination would not generate any centrifugal force as it spins.
Fig. 2-1-15 Two types of toolholders with two-face conical tapers. A (Stanley Sheppard Co.) B (HPI/Nikken)
Importance of Concentricity
High-speed milling is generally low-depth-of-cut milling. The cutting load is lighter than in conventional milling. Therefore, the potential variation in load introduced by cutting tool runout becomes more significant by comparison.
Concentricity is also important because of the cutting tool materials used in HSM. These must offer high wear resistance and heat hardness, but they often achieve this at the price of low toughness. Carbide tooling, for example, will chip or fracture more easily than steel tools. More exotic materials, such as diamond, are more brittle still. At high speeds, evenly distributed loads resulting from low runout can be essential to achieving acceptable tool life with these materials.
HYDRAULIC TOOLHOLDERS
A hydraulic toolholder uses a reservoir of oil to equalize clamping pressure around the tool. Turning a screw increases the pressure on this oil, causing an expanding sleeve to grip the tool shank. This type of toolholder is used in many shops because it centers the tool well and is more versatile.
Fig. 2-1-16 Concentricity and balance are important to a successful high-speed machining. (Modern Machine Shop)
Researchers sampled a variety of collet, side-lock, and hydraulic toolholders, Fig. 2-1-17. The horizontal arrows show the range of tool runout errors measured on these toolholders. The curves show the effect of this runout on the average life of tools (in this case, drills) made from conventional carbide and from a carbide grade engineered for higher toughness.
SHRINK FIT TOOLHOLDERS
A shrink fit toolholder is the best toolholder because gripping force is higher, there are no moving parts, and the balance is near to perfect. It works in conjunction with a specialized heater and takes advantage of thermal expansion and contraction to clamp the tool. At normal shop temperature, the bore in which the tool locates is slightly undersize compared to the tool shank size. Heating the toolholder enlarges its bore to allow the tool shank to be inserted. As the toolholder cools, the bore shrinks around the tool shank to create a concentric and rigid clamp.
TOOLHOLDERS FOR BALANCE
Balance is important to an efficient machining operation. Some toolholders, such as shrink-fit holders, have good balance while others such as collet holders can be balanced. Most of these holders provide enough balance for many HSM processes. Balancing should be performed at the speed the tool-holder is to be operated.
BALANCEABLE HOLDERS
A balanceable toolholder is used in conjunction with a balancing machine, Fig. 2-1-18. The machine measures the unbalance in the tool/toolholder system that contains counterweights that can be adjusted to compensate for the unbalance.
Fig. 2-1-17 A comparison of toolholder performance. (Modern Machine Shop)
Fig. 2-1-18 A toolholder balancing machine. (American Hoffman & Lyndex)
Importance of Balance
Not all HSM processes demand the best achievable balance. Unbalance will cause vibration, but the cut also causes vibration. And the force from unbalance may be insignificant compared to the force from the cut itself. The important question is whether or not the unbalance affects the process.
Possible clues that better balance is needed include unacceptable surface finish or tool life, or problems meeting tolerance for characteristics such as hole roundness or trueness.
CUTTING TOOLS
In high-speed machining, the cutting tool may set the speed limit, Fig. 2-1-19. Many machining centers today run at speeds beyond what today’s tooling can put to use without premature failure or excessive wear. In a process optimized for high-speed machining, the tool will probably determine just how fast the cut can be taken.
Fig. 2-1-19 In high-speed machining, the cutting tool usually sets the limit. (Modern Machine Shop)
Tool Rigidity
High spindle speeds increase the severity of vibration at the tool tip. To protect tool life and surface quality, favor more rigid tools. Many times it is more efficient to rough with a smaller tool to get close to finish size and then finish with the final tool. For the best rigidity when using end mills:
▪Use the shortest tool possible, Fig. 2-1-20.
▪Favor a tool with shorter flutes (and therefore a larger and more rigid central core).
FINE GRAIN CARBIDE
Most applications call for carbide tooling and the grade should be chosen not just for its hardness (resistance to wear), but also for its toughness (resistance to shocks). High-speed machining is often high-shock machining; impact, vibration, and temperature changes are more dramatic at higher speeds. A tool with higher toughness is less likely to chip or crack as a result of these shocks.
A good compromise between hardness and toughness comes from carbides with small grain sizes. Many fine-grain carbides available today deliver improved toughness, with little change in hardness compared to coarser grades, Fig. 2-1-21.
TiAIN and TiCN Coatings
TiAIN is an effective coating for a wide variety of HSM applications. The coating delivers a variety of benefits to extend tool life, including:
▪High-temperature wear resistance – High-speed machining is often high-temperature machining. The cutting tool must be chosen not just for its wear resistance, but also for its ability to retain this wear resistance at higher temperatures. TiAIN protects the tool by acting as a thermal barrier. The coating is about 35% more heat resistant than titanium nitride (TiN).
Fig. 2-1-20 Use short cutting tools to reduce vibration at the tool tip. (Modern Machine Shop)
Fig. 2-1-21 Fine carbide grades provide a balance between hardness and toughness. (Guhring)
▪Lubricity layer for chip removal - High-temperature cutting with TiAIN encourages the formation of a useful outer layer of aluminum oxide. This layer is both hard and slick. While the hardness helps with wear resistance, the slickness lubricates the hot chip to help it slide away without adhesion or heat transfer.
▪Abrasion resistance - TiAIN’s abrasion resistance makes it effective for machining graphite.
Because the coating performs effectively at high temperatures, tools with TiAIN are generally run dry, Fig. 2-1-22A. TiCN (Titanium carbon nitride) is a less expensive coating suitable where hardness and speed are not at the highest levels, Fig. 2-1-22B. For a ball-nose tool, TiCN may be appropriate when workpiece hardness is less than 42 Rc and cutting speed is less than 800 sf/min. At these conditions, use of coolant is acceptable.
USE OF COOLANT
High-speed machining often means dry machining. The mechanics of the high-speed cut can convey some heat away. As for the rest, a consistent high temperature may be better for the tool than the widely varying temperature that coolant can bring about.
Coolant does have a role. Use it where lubrication is necessary to protect either the surface finish or the tool, Fig. 2-1-23.
MATERIALS
As newer materials are developed, manufacturers look for methods of machining them faster. It is always wise to follow the material and cutting manufacturer’s recommendation when cutting new materials or using new cutting tools. The following are general guidelines for a few materials:
▪Aluminum – Machine speed should be at least 10,000 sf/min. with a chip thickness of not less than .001 in. to prevent built up edge from forming on the tool that results in premature tool failure.
Fig. 2-1-22 Coatings provide abrasion resistance and lubricity to carbide tools. (Balzers Tool Coating, Inc.) (A) TiAIN coating (B) TiCN coating
▪Compacted graphite iron – Harder than previous cast irons, is more difficult to machine and requires a sturdy machine to support the greater cutting forces.
▪Cast irons – Machine aggressively at speeds up to 3,500 sf/min. with silicon nitride, CBN, or diamond tools.
▪Composites – Use negative cutting tools so that most of the forces applied go into the tool and not the material.
▪High-temperature alloys – Use a coated carbide or CBN tool that cuts well at 500 r/min. as well as 15,000 r/min. to avoid using two machines. Cutting these alloys requires higher horsepower and better tooling.
DRY MACHINING
A steady high temperature at the cutting edge can be better than temperature that fluctuates because of coolant. Coated carbide tools can stand up to the heat, but intermittent cooling can cause carbide to crack. Also, TiAIN coating may perform better when hot, that’s why HSM processes are often run dry.
HSM may even create its own heat-management effect. Fast cutting at a light depth encourages heat to leave the work zone with the chip instead of building up in the part, Fig. 2-1-24. One result is that chips may be harder than the parent material. Therefore, protect the tool during dry machining by using forced air to blow these hard chips away.
USE COOLANT FOR LUBRICATION
The cooling effect of coolant may not be well suited to HSM, but the lubrication effect may be valuable. Use coolant for gummy materials such as aluminum or soft stainless steel to help the chip slide along the flute without adhering. In these materials in particular, consider coolant when taking cuts near the tip of a ball-nose tool where sf/min. approaches zero. When the cut is very light, hot material can be welded to this region of the tool, affecting finish quality. Coolant helps minimize this effect.
Fig. 2-1-23 Coolant can be used to lubricate the tool and protect the surface finish. (Modern Machine Shop)
Fig. 2-1-24 A model showing that most of the heat is carried away with the chip. (Third Wave Systems)
SPEED, FEED RATE, AND DEPTH OF CUT
Tool life and tool performance in HSM are determined largely by how much load there is on the tool. Because speed increases the effect of small differences resulting from factors such as toolholding, tool path and control, this will vary from process to process. How fast each process can be machined may require that the starting point should be at the lower range and increased until ideal machining conditions are reached.
The following are general guidelines when using HSM with a ball-nose tool for finishing operations:
▪Speed - At or near maximum spindle r/min.
▪Feed rate – Use light cuts at chip load equivalent to that of lower speeds.
▪Depth of cut - No more than 10% of cutter diameter, even less for harder materials.
Note: It is important not to exceed a tool’s maximum safe speed. Always follow safety precautions appropriate to higher speeds.
SAFETY AT HIGH SPINDLE SPEEDS
Centrifugal force at high spindle speeds can turn any loose insert, screw, or tool fragment into a dangerous projectile, Fig. 2-1-25. Use the following precautions when machining at high spindle speeds:
▪Do not exceed a tool’s maximum spindle speed rating.
▪Check tools and toolholder components regularly 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 CNC with look-ahead capability will try to protect the tool, work, and machine from the effects of sharp changes in direction at high feed rates by slowing the feed in advance of the turn, Fig. 2-1-30. This slowing down sacrifices efficiency and may visibly affect the surface of the part. To keep the tool path fast and effective, avoid slow-downs by making direction changes more gradual. There are a variety of ways to machine with smoother motion such as rounding corners, smoothing reversals, and machining in circles.
Another approach to keeping the feed rate high does not involve direction changes, but instead changes in the feed rate. Feed rate optimization may allow the program to keep a higher average feed rate where the profile of the cut changes often.
Fig. 2-1-30 In high-speed machining, the feed rate should be kept as fast as possible. (Modern Machine Shop)
SUMMARY
▪HSM uses high spindle speeds, high feed rates, and light depths of cut to increase productivity, reduce lead time, reduce warping, increase part accuracy, and improve surface quality.
▪High-speed machining begins at 12,000 surface feet per minute (sf/min.) and may be as high as 18,000 sf/min. and feed rates of 600 in/min. when machining aluminum.
▪The key factors that affect the efficiency of a HSM system are the machine tool, the controller, spindle, toolholder, cutting tool, and programming.
▪The CNC control, cutting tool, machining center and other components must be designed with the goal of using the higher spindle speed productivity.
▪In a toolholding system consisting of the spindle, toolholder, and cutting tool, the toolholder is the most important link because it has the greatest effect on the overall concentricity and balance.
▪A balanced toolholder is critical for producing high-quality surface finishes, extending spindle life, and reducing or eliminating vibration that can affect the metal-removal process.
For more information on HIGH SPEED MACHINING see the Websites: www.turchan.com www.mmsonline.co
