thumbnail group

Connect With Us:

ME Channels / Controls & Software

Unleash Your CNC's Power


You can do more with what you already have

By James R. Koelsch
Contributing Editor 

If you're like most machine shops, you want to cut faster and hold better accuracy on your machining centers—without having to invest much money. Well, the means for doing just that could already be sitting in your shop. One of the best-kept secrets in the industry is that most modern CNCs contain many performance-enhancing features that builders of general-purpose machines often don't use. All you need to do is turn them on.

"CNCs have a lot of capability that's not taken advantage of," says Bill Griffith, CNC product manager, GE Fanuc Automation North America Inc. (Charlottesville, VA). "You can hire a service engineer to set them up for you. Sometimes maintenance engineers learn about some features in the training classes that they take."

The availability of these performance enhancements varies widely with the make of the CNC and its manufacturer's marketing strategy. Some manufacturers, for example, activate all of the features that they offer, making them available to users from the outset to avoid "optioning" them to death. You just need to learn to use them. Others, however, price their products based on the active features, requiring their customers to pay only for those features that they use. So if the builder of your machine did not activate a feature that you might find useful, you will need to buy it.

Although the cost of such features usually runs between $900 and $2000 each, it varies by manufacturer and type of feature. Sometimes the purchase is simply a matter of giving the CNC manufacturer your credit card number over the phone, and receiving an activation code that you punch into the CNC. Other times, however, a technician needs to come to the machine to activate and tune the feature, and perhaps even load a missing piece of software. In these cases, you'll need to add the cost of the service call, which usually requires from a few hours to a day.

Keep in mind, however, that using these hidden features isn't always just a matter of turning them on. Sometimes there is a tuning, or commissioning, process. Other times, you need to tweak cutting programs and internal software to account for the changes made by a feature. "You have to be aware of what you are doing to enhance your machine, because it might affect how the machine will operate," says Christian Kuhls, CNC product manager, Siemens Energy and Automation Inc. (Elk Grove Village, IL).

An example is the motion-synchronous actions, or synchronized actions, feature in Siemens' CNCs. This feature allows users to program instructions— such as sending output of auxiliary functions to the PLC, writing and reading of real-time variables, making on-line tool offsets, taking measurements, and calculating of function values—that are processed synchronously with the interpolation cycle. The goal is to complete tasks or to provide data in time for use. Since you integrate these actions into the machine and coordinate them with the tool motion, you might need to adjust them if any features change the machine.

To help users sort through the various features that are hiding in the CNC and to decide which would boost the performance of their machines the most, GE Fanuc's Griffith suggests organizing them into a kind of hierarchy—one that puts sound mechanics at the base. Although software and electronics might mask some mechanical defects, they cannot make an unsound machine sound. The hierarchy then builds on the base of sound mechanics, beginning with servo and positioning adjustments, continuing with features that enhance the machine's acceleration (and deceleration, which is nothing more than negative acceleration) and programming, and ending with those that add functionality to the machine.

At the lowest level, adjusting servo and positioning parameters, the first order of business is tuning the velocity loop. The process involves determining the natural frequency of the machine, which tells you the performance limits of the machine and lets you set resonance filters, velocity loop gain, feed-forward coefficient, and position gain accordingly. GE Fanuc has software called Servo Guide that leads users through this initial tuning process.

"Servo-tuning functions like feed-forward control are in every CNC, but aren't always used," says Griffith. "The feed-forward function more or less skips the position loop and sends the command directly to the velocity loop of the servo system." By bypassing the slower position loop, the feature hastens the CNC's response to any deviations from the programmed toolpath, allowing the machine to react to corners and contours much faster. Consequently, feed-forward control reduces any position errors that would result from servo-processing delays when cutting at high feed rates.

A feature called nanometer command interpolation allows Fanuc CNCs to send commands to the servo system in increments that are a thousand times smaller than before. These tiny, nanometer-size command increments not only improve accuracy by moving rounding error to smaller decimal places, but also make acceleration smoother, which allows you to cut at faster rates.


One performance-enhancing feature on GE Fanuc's CNCs filters vibration at the frequencies that generate strong resonance on a particular machine. (Click on image to enlarge)

Griffith emphasizes that this feature is not a function of the positioning accuracy of the machine. "It is strictly a command unit between the CNC and the servo system," he explains. "So it doesn't need nanometer feedback on the position feedback loop." It does, however, need high servo responses to be able to handle the amount of data being processed. For this reason, GE Fanuc's CNCs have high-response velocity feedback that samples velocity from the motor every 64 nsec.

If you are looking for a way to hold tighter tolerances and create finer finishes, you might check your CNC for error-compensation features. Many CNC manufacturers have equipped their products with optimization features that run tests to measure mechanical errors, power transmission faults, and measurement errors, and to compensate for them. "Interpolatory tests, for example, check the contour accuracy of your axes, compensating for any gap in their ability to return the tool to a particular point in space," says Siemens' Kuhls.

Besides performing these interpolatory tests for leadscrew error and beam sag, Siemens' CNCs also compensate for temperature changes, backlash, and friction, and provide dynamic feed-forward control and electronic counterweights for drives. Because these tests take only about 5–10 min to run and generate optimum compensation coefficients, Kuhls recommends running them periodically as part of a maintenance schedule to compensate for normal wear and changing conditions.

"If you do it on a regular basis, you can identify faults much earlier and schedule maintenance based on these values," he says. "You'll be performing maintenance based on the actual status of your machine, not on how long it has been operating."

Siemens' CNCs also can perform vibration analyses, and help the user filter and damp internal noise. Kuhls reports, however, that this test is more involved than the others. It not only needs much more time, but also requires a fair amount of expertise. Consequently, he recommends hiring an expert to perform it.

A machine's acceleration profile is the next level in the hierarchy of hidden features. These options can shave milliseconds off each inflection point where an axis changes its rate of acceleration. Because a typical contour has thousands of blocks, the time savings can be quite large when you add them up, especially on large parts. Moreover, controlling changes in velocity and acceleration better can reduce vibration and shock that can damage a machine at high speeds.

One way to squeeze time from toolpaths is to use a more efficient acceleration profile, which CNC manufacturers allow users to change through a feature called the acc/dec control. "Many builders set their machines' acc and dec control to follow an exponential curve during acceleration," explains GE Fanuc's Griffith. "Linear and bell-shaped curves are available too. Each has its advantages and disadvantages, but an exponential curve is the lowest base feature, and will give you the least performance."

Of these profiles, the bell-shaped acceleration curve is usually best because it avoids shocking the machine. "A linear acceleration is very sharp," Griffith notes. "A lot of machine tool builders don't build machines that are rigid enough to handle a truly linear acc and dec. If the machine can handle a linear acceleration, though, linear is just as good as bell-shaped."

If the acc/dec control feature is activated, anyone who knows the basics of the machine and has the experience can tune the machine in about an hour. Doing it right, however, requires a ball-bar test. "An experienced person can tune the gains, adjust the feed-forward coefficient, and set acc/dec profile in an afternoon," says Griffith.

Another oft-ignored feature is jerk control, a feature that controls shock from inertia, friction, and internal play by smoothing abrupt changes in acceleration. According to Griffith, true jerk control is the first derivative of acceleration at points of change. It is not a bell-shaped acceleration curve, which some CNC vendors called jerk control in the past. The advantage of true jerk control is that it is better at smoothing jerks. "It reduces shock so you can lower acc/dec constants and accelerate faster," says Griffith.

GE Fanuc offers another acceleration-improving feature called Optimum Torque. As the name suggests, this feature adjusts acceleration based on the speed-torque curve of the motors to ensure that the machine is using as much of its cutting capacity as it can. Because an intimate knowledge of the motor, amplifiers, and control loops is necessary to make this feature work, it usually requires that the CNC, drives, and motors come from the same manufacturer.

A good application for this feature is optimizing machines that cut parts that differ widely in weight. "If you set the machine for a very heavy part, you're stuck with that acc and dec," says Griffith. "With Optimum Torque Acc/Dec, the machine can accelerate faster without any adjustments when we put a light part on the machine. Because the CNC accelerates based on the torque of the motor, you no longer have to set the machine for the worst-case scenario. Now, it will adapt."

Tools for programming toolpaths are the next level in the hierarchy of hidden features. CNC manufacturers build some kind of programming software into their products, and offer a variety of alternatives as options. One is a basic CAD/CAM system called profile editors for creating electronic "blueprints" on the CNC's screen. Upon creating a profile, the operator simply saves the profile or blueprint as a program, a process that generates G-codes automatically.

This ability can come in handy for a shop cutting a family of parts containing four profiles, according to Todd Drane at Fagor Automation Corp. (Elk Grove Village, IL). It could let production bypass the CAD/CAM department and the associated trial and error of creating a file offline. Because loading a new profile using a profile editor such as the one Fagor offers can take between one and three minutes, depending on the part's complexity, downtime for program changes is much shorter than typically required for importing and programming profiles from the CAD/CAM system.

Many CNCs also have a conversational operating system available to give the operator the option not to work with G-codes. "We recommend that users consider using one in most situations where part programs are created at the machine," says Drane. The operator simply selects the operation that he wants to perform and fills in the blanks on the graphics that appear on the screen. This lets him simulate cutting graphically or execute the program without having to know G-codes.

When using Fagor's CNCs, the operator makes his selection by pressing the key on the keyboard containing the icon that depicts the operation that he wants to perform. Drane recommends activating this feature when you order the CNC, because the keyboard needs the keys containing the icons.

Although some kind of programming software is typically standard issue on CNCs, the tools for importing files are not always. Heidenhain Corp. (Schaumburg, IL), for example, puts a DXF converter in its CNCs, but does not turn it on. "Not everybody needs it," explains Chris Weber, product manager for controls. If you are someone who does, contact Heidenhain, pay the fee, and get the code that activates the option.

CNCs also often contain programming tools for customizing the user interface for the particular jobs that the user has or for the particular tasks that management expects of the operator. These customization tools usually fall into two groups or levels. First is an elementary level that Siemens calls its expanded user interface wizard for adding setup instructions and other screens. "It enables you to develop your own screens just with ASCII files," says Kuhls. "We also have options that let you generate complex screens in higher languages like C++ or Visual Basic." This higher level of customization allows users to create screens that pull information from others, so operators need not flip through several screens to get the information that they need.

Tools for efficient and safe motion form yet another level in the hierarchy. Bosch Rexroth Corp. (Hoffman Estates, IL) has a fast auxiliary-processing feature for activating tool changers, coolant pumps, clamps, and other auxiliary devices quickly. It's especially handy on jobs that require several tool changes or need selective use of high-pressure coolant. After configuring an auxiliary function as a "fast" function in the setup page, the programmer inserts the function early to ensure that it is on.

"Before the motion block where the function must be on—confirmed by the CNC logic controller via a switch, etc.—the user programs an auxiliary function check," says Bosch Rexroth's Karl Rapp, branch manager for the machine tool industry. "Using this method avoids unnecessary stopping of the NC-block execution, and could reduce machining time." He emphasizes the need for diligence in ensuring that the feature activated or deactivated by the auxiliary function is truly finished before going to the next motion block.

Most CNCs also contain tools for altering the programmed feed rates as conditions permit to boost productivity. A feature in Heidenhain's CNCs, for example, adjusts the feeds automatically based on the tolerances that you set for each feature in a cut. "If you want to cut at 300 ipm [7620 mm/min] yet want to hold a micron around a corner, the cycle will override programmed feed rate and decelerate automatically as it approaches the corner so it can hold tolerance," says Weber. In Heidenhain's case, the feature is free, but needs activating.

GE Fanuc takes this ability a step further with its Machine Condition Select feature. In addition to adjusting the feed rates, the feature also switches the servo gains and other parameters based on the tolerance and finish requirements. It allows users to identify as many as 10 cutting conditions, set as many as 12 parameters for each of those conditions, and have the program load them into the CNC on the fly to cut at optimum settings. "It allows you to have a roughing cut that is not as accurate, but much faster, and have a finishing cut that is very accurate but running at a feed rate corresponding to the accuracy," says Graham.

Heidenhain also offers a paid option called Dynamic Collision Monitoring that protects the machine automatically from collisions, no matter what the program tells the machine to do. Machine tool builders can use this feature to create maps of their machines' work envelopes and link them to the kinematics of CNCs. "The controller knows where everything is and will not let you move, say, the spindle into the toolchanger," says Weber. "Even if you try to move the spindle with the handwheels to crash into a tool probe, the control will prevent you from doing it."

Because the commissioning of this feature is involved and requires a measure of expertise, it is a tool intended mostly for machine builders or integrators. Nevertheless, it is an option gaining the attention of users of five-axis machining centers. "The odds of crashing into something are fairly slim on a three-axis machine," explains Weber. "But it becomes an issue on five-axis machines capable of tilting and swiveling," in addition to moving along the three conventional linear axes.

GE Fanuc has developed a feature called Machining Point Control for damping vibration as large machines move through rapid traverses and cuts. It reads vibration at the tool tip or in moving members with a three-axis accelerometer attached to the machine much like a linear scale would be. The vibration signal goes through the velocity loop of the CNC, which adds a negative error adjustment in the opposite direction. "It damps the true vibration, not the predicted vibration," says Griffith.

He expects the first applications to be on the large machines making wing and fuselage segments in the aerospace industry. "In the past, the only way to damp vibration was to filter it through the servo system based on the machine's natural frequencies," he says.

At the highest level of the hierarchy of hidden power are the features on many of today's CNCs for streamlining the adding of functionality. Heidenhain, for example, makes its CNCs in only five and 10-input models. Machine tool builders pay for only those axes that they use, and let the others lie inactive. Consequently, CNCs often have the capacity to run more axes. So someone who has a machine using only six of the inputs on a 10-input CNC can pay a fee to activate that dormant axis to add, perhaps, a rotary table.

Activating the axis is a simple process that requires a lead time of about a day. The user places the order through the local distributor, who then relays the CNC's system identification key (SIK) to Heidenhain. "Once we have the SIK, we know everything about the machine and can send the appropriate activation code to the customer by e-mail," says Weber. "The customer punches in the code, and his axis lights up." The CNC is then ready for the integrator to attach the table and commission the servo loops.

Another advantage of the SIK is that a user can transfer the CNC's setup parameters to another controller. If a worker were to drive a fork-lift truck into the machine and ruin the CNC, then a technician could pull out the hard drive and the card containing the SIK, and plug them into a replacement CNC. "It brings along all of the setup and commission parameters," says Weber. "The new unit now is the same as the old one."

Users also can expand the functionality of their machines by adding touch probes. Because Heidenhain makes these devices, it equips all of its CNCs with the software and communications ports necessary for installing and using on-machine probes. "Our controller has two dedicated inputs, one for spindle probes and the other for tool probes," says Weber. Because the macros for probing are already loaded on the controller, the cycles light up on the screen when you turn them on. The documentation is available for downloading for free from Heidenhain's Web site. The only cost associated with this feature is buying the probes.

Before you can begin probing, however, you have to commission the feature to set the approach speeds. "For example, I might want the machine to rapid traverse until the probe is within 10 mm of the part, and then slow the feed to move closer and do the actual triggering," notes Weber. He says that the commissioning is a fairly simple process that takes about two hours.

The probing software offered by Heidenhain and other CNC manufacturers like Fagor includes cycles for manual part setup and automatic inspection of both cutting tools and parts. Canned probing cycles can greatly reduce setup time too. "Users can automatically find fixture offsets, hole centers, and fixture angle offsets, and load these points directly into the zero-offset tables," says Fagor's Drane.

He also recommends to shops using on-machine probes a digitizing feature that they can activate in Fagor's CNCs. This feature can create a program automatically after sweeping a sample part with a probe in either concentric circular or in rectangular "cornrow" patterns. "A user simply fills in the blank of the pattern that he or she wishes to digitize," says Drane. He estimates that the typical user can create a digitizing cycle and begin executing it within three minutes.


This article was first published in the September 2006 edition of Manufacturing Engineering magazine. 

Published Date : 9/1/2006

Editor's Picks

Advanced Manufacturing Media - SME
U.S. Office  |  One SME Drive, Dearborn, MI 48128  |  Customer Care: 800.733.4763  |  313.425.3000
Canadian Office  |  7100 Woodbine Avenue, Suite 312, Markham, ON, L3R 5J2  888.322.7333
Tooling U  |   3615 Superior Avenue East, Building 44, 6th Floor, Cleveland, OH 44114  |  866.706.8665