Product Corner: Two Operators’ Guides to help operators learn to run CNCs

• Machining Center Operator’s Guide

• Turning Center Operator’s Guide

When it comes to sheer numbers, CNC operators make up the greatest percentage of CNC people.  For this reason, the position of CNC operator is the most difficult one to keep fully staffed. Most companies find it difficult to find and hire qualified people – and are training new people from scratch. These two self-study manuals can really help bring new people up to speed.

They are designed to help entry-level CNC people learn what it takes to run CNC the two most popular forms of CNC machine tools. We begin by discussing some of the basic machining practice skills a CNC operator must understand, including blueprint reading, tolerance interpretation, gauging skills, and machining operations. We then present the tasks required to setup and run a CNC machine. We place heavy emphasis on what it takes to hold size during a production run (measuring a workpiece, determining if dimensions are to size, and how to adjust when they’re not).  Learn more about how these guides can help!

Top of page

Instructor Note: The most important thing a CNC operator must know

Most companies expect a lot from their CNC operators. Common tasks include:

• Loading and unloading workpieces

• Activating and monitoring the CNC cycle

• Measuring workpieces and reporting findings to an statistical process

• control (SPC) system

• Making adjustments required due to tool wear

• Replacing dull tools

• Keeping the machine and work area clean

Every one of these tasks, of course, is very important, and it could probably argued that any one of them is the most important – for without a mastery of each task, a CNC operator will not be successful.

Maybe a better question might be “Which task does an operator tend to struggle with the most – when mistakes can lead to wasted time, scrap parts, and possibly dangerous situation?” Again, several of the related tasks may come to mind. But the one we’d like to stress is Making adjustments due to tool wear.

Since turning centers incorporate many single-point cutting tools, they tend to require the most in the way of workpiece sizing. However, machining centers also require their share of sizing adjustments. In any event, a CNC operator must be able to determine whether a measured attribute is within its tolerance band. Since this is such a basic task, experience, shop people tend to take the related skills for granted – and sometimes assume that everyone (including entry level CNC operators) can do them.

Measuring

The first related skill an entry level operator must master is accurately measuring workpiece attributes with the gauging tools your company uses. This can take a lot of practice, especially with variable gauges that have Vernier (or similar) scales. For this reason, more and more companies use gauges with dial or (better yet) digital displays.

Measuring accurately requires a certain “feel”. Once a person is taught how to use one of your gauges, they must practice to master it. One way to get started is to use known sizes for measuring. For example, use a set of gauge blocks to simulate workpieces.  If the operator know the thickness of a gauge block is supposed to be 0.500 inch, for example, they’ll be able to experience the feel of the gauge when it displays 0.500 inch. This is mandatory when measuring actual workpiece attributes.

Evaluating measured values

Assuming a CNC operator can accurately measure workpiece attributes, next think about what must be done in order to determine whether a given workpiece attribute is within its tolerance band. Consider a “simple” 2.0 inch turned (external) diameter machined on a turning center. How is the tolerance specified? It could be done in at least three ways:

• With a plus/minus tolerance specification (2.000 +/- 0.002)

• With an uneven tolerance specification (2.001 +0.001 -0.003)

• With the high and low limits (2.002 / 1.998)

Even for this simple example, it can be difficult to get across the point that, in order for the turned diameter to be acceptable, the operator’s measured dimension must fall between 1.998 and 2.002 inches. Again, this may seem elementary to any shop person, but it will be a new concept for most non-manufacturing people. It will take practice to master.

Remember, we’ve shown a pretty simple dimension and tolerance example. Determining the high and low limits is pretty easy in our case. But consider a dimension and tolerance of 1.8324 +0.0004 -0.003. Even experienced shop people may have to think about this one for a bit before they can determine the mean value and high/low limits. A newcomer may have to use a calculator.

As you begin teaching people how to hold size on CNC machines, remember that  this is a task they must be able to perform flawlessly and consistently – based upon the dimensioning and tolerancing methods you use. You can have them practice by giving them problems like this to solve:

• Dimension is 2.125 +/- 0.004. The workpiece attribute you measure is 2.123.  Is the measured value within the tolerance band?

The target value

Next, CNC operators must understand that when a measured workpiece attribute is not within its tolerance band (and often even when it is), an adjustment must be made. Making an adjustment first requires a person be able to determine the target value. That is, the dimension the operator is shooting for with the adjustment. Many companies have their CNC operators target the mean value of the tolerance band – and this may be just fine in the beginning.

(But remember, when you target the mean value, you’re only working with half the tolerance band – and adjustments will be required twice as often. Based upon the direction of workpiece-attribute growth caused by tool wear, many CNC operators will target a value closer to the high or low limit – whichever provides the longer period of unattended operation. This concept, however, may be a little difficult to relate to entry-level operators. The more important point is that they will have to know the target value before an adjustment can be made.)

Based upon your company’s methods, you must ensure that entry-level operators can accurately and consistently determine the target value. Again, coming up with exercises shouldn’t be too tough:

We target the mean value of all tolerance bands. Based upon the following dimensions, what is the target value?

• 2.000 +/- 0.002

• 2.375 +0.001, -0.003

• 1.4378 / 1.4373

When to make an adjustment

CNC operators must know when adjustments are required. Companies vary with specifics, but the concept remains the same. Of course the operator will make an adjustment when a measured workpiece attribute is not within its tolerance band (and the current workpiece is scrap). They must know not to run any more parts until the adjustment is made (don’t assume they know this).

More commonly, CNC operators will be making adjustments as the growing or shrinking workpiece attribute draws close to a high or low limit. Explain that this growing or shrinking is caused by tool wear - and is especially common with single point tools. As tools wear, more and more material will be left on the surface/s machined by the tool. As more and more material is left on the surface, external surfaces (like turned diameters) will grow and internal surfaces (like bored holes) will shrink.

So a turned diameter that starts out at precisely 2.000 inches in diameter will grow as more and more workpieces are machined. After fifty parts, this dimension may be 2.0003 (it has grown by 0.0003 inch). After fifty more parts, it becomes 2.0007. And so on. Eventually the tool will become completely dull and will require replacement, but a lot of growth (or shrinkage) can occur before this is necessary. In most cases, and especially with tighter (smaller) tolerances, the workpiece attribute will grow or shrink out of its tolerance band long before the tool is dull.  This means several adjustments will often be necessary during a tool's life.

So, exactly when should the adjustment be made? Again companies vary with what they tell operators to do, and of course, you’ll relate your methods to your new CNC operators. Most have a ten or twenty percent rule-of-thumb. When the surface grows to within ten or twenty percent of a tolerance limit, an adjustment will be made. Better stated, when a 2.000 +/- 0.001 tolerance grows to 2.0008 or 2.0009, an adjustment will be made.

How much to adjust

CNC operators must be able to determine the amount and direction for the required adjustment. Explain that the adjustment amount is simply the difference between the measured value and the mean value. If an operator measures a turned diameter with a target dimension of 2.000 inches as 2.002, the adjustment amount will be 0.002. Again, you can easily come up with exercises for determining adjustment amount.

Polarity of adjustment

Explain that in some cases, the adjustment will be positive and in others, it will be negative. Determining polarity requires an understanding of the machine’s axes – as well as their polarity. So be prepared to explain which way is plus and which way is minus for each axis.

Fortunately, many turning center adjustments are very simple: If a turned or bored diameter is too big, the adjustment will be negative. If it is too small, the adjustment will be positive (for most turning centers). Again, be prepared to explain polarity of each kind of adjustment your operators will be making.

And again, develop exercises to confirm entry-level operators understand:

• We target the mean value for all dimensions. Dimension is 2.000 +/-0.001. Measured value is 2.0008. What is the adjustment amount and polarity?

What must be adjusted?

In rare cases, the cutting tool itself must be adjusted. Consider, for example, a boring bar used on a machining center. A mechanical dial controls the precise diameter that the boring bar will machine. If the measured hole size is too small, the dial will be turned in one direction. If it is too big, the dial will be turned in another. And mechanical linkages precisely move the boring bar insert to make a bigger or smaller diameter.

In most cases, adjustments will be made in offsets – so be ready to explain what they are and how to access them. Explain that offsets are referenced by a number – offset one, offset two, and so on. Also explain if your offsets contain more than one value (length and diameter for a machining center for example – or X and Z for a turning center).

CNC operators must know which offset must be adjusted - and if the offset contains more than one register, which register is involved. Explain that most programmers will make the offset number correspond to the tool station number – so if the operator knows which tool machines a surface, they’ll know the offset number that contains the adjustment values.

(Even this concept is difficult to relate. It can be hard for an entry-level operator to determine which offset must be adjusted. For reason, more and more companies are including offset information in the production run documentation that goes along with the job.)

Unfortunately, practicing this can be more difficult. Take newcomers out to your currently running machines and show them how to determine which tool machines each surface and how to determine the related station numbers and offset numbers. Have them tag along with experienced operators to see it done first hand.

Top of page

Manager's Insight: Separating cutting and non-cutting time in a CNC cycle

Managers often want to know the percentage of time a machine is actually cutting something in a CNC cycle, but trying to calculate cutting versus non-cutting time can be difficult. But by running two CNC cycles (one without a workpiece) there is a relatively quick and definitely easy way to separate cutting time from non-cutting time.

First of all, let’s define cutting time and non-cutting time:

• Cutting time is time when the machine is in a cutting mode (G01, G02, G03, etc.).

• Non-cutting time is everything else (rapid [G00] motions, tool changes, indexes, etc.).

Admittedly, some of the time we attribute to cutting time is related to times when the machine is feeding but not cutting (feeding into and out of a cut). The amount of rapid approach distance, of course, affects how much time is taken during these motions.

First of all, run and time the cycle in the normal fashion – with the feedrate override switch at 100%. You can actually run a part during this time. For the formula that we’ll show, we’ll call this normal feedrate run time.

Second, run and time the cycle with the feedrate override switch set to 200%. You cannot, of course, run a workpiece during this cycle. We’ll call this the double feedrate run time.

With the two times available, apply these two simple formulae to determine cutting time and non-cutting time:

• Cutting time = (normal feedrate run time minus double feedrate run time) times two

• Non-cutting time = normal feedrate run time minus cutting time (that you just calculated)

Here is an example. Say your normal feedrate run time is 17 minutes. The double feedrate run time is 9.5 minutes. (17 minus 9.5) times 2 is 15, meaning fifteen minutes of the cycle is cutting time and two minutes of the cycle (17-15) is non-cutting time.

This works because only the cutting motion feedrate is doubled when you turn the feedrate override switch to 200%. For this reason, the difference between the normal feedrate run time and the double feedrate run time is half the cutting time.

Top of page

G Code Primer: Restarting after breaking a tap

One of the most frustrating problems a CNC operator can have is breaking a tap in the middle of taping many holes. The broken tap, of course, must be removed from the workpiece and the hole repaired (re-tapped), but it is not often feasible or desirable to repair the hole during the CNC cycle. Most companies will leave the broken tap in the hole and will remove it and re-tap the hole by hand after the workpiece comes out of the machine.

But a major problem still exists. How do you tap the rest of the holes that were to be tapped after the tap broke? Consider, for example, having 200 holes to tap. On the 150th hole, the tap breaks. This means, of course, that there are still 50 holes to tap (after replacing the tap).

The operator must have a way to run the tap in these holes. One way is to rerun the entire tapping cycle, but this would mean re-tapping 150 holes. And if the broken tap remains in the hole, what then? Some operators will place a block delete code (slash code) in at the beginning of the command that taps the hole with the broken tap. If only a few holes must be re-tapped, this may not be too bad an idea. But if there are many holes – and especially when the possibility exists that a hole will be cross threaded if the tap reenters each hole (machines without rigid tapping are notorious for cross threading), a better way must be found.

Unfortunately, my suggestion requires a good understanding of manual programming and rerunning tools. In essence, we’re going to be modifying the program in such a way that the tapping cycle will be instated for the first hole, but the first hole will not be tapped. We’ll also ensure that the tap begins at a high enough Z location that the tap will remain over the remnant of the broken tap if it happens to go near it. Finally, we’ll need to confirm that the restart hole (where you want the tap to continue) has both an X and Y coordinate (many of the commands that specify hole locations have only one coordinate), and that the Z surfaces (Z and R) are appropriate.

Here is an example of how the program must be modified:

• Original program:

• (3/8-16 TAP)

• N405 T08 M06

• N410 G54 G90 S400 M03 T01

• N415 G00 X2.5 Y1.0

• N420 G43 H08 Z0.1

• N425 M08

• N430 G84 R0 Z-1.0 F25.0

• N435 Y1.5

• N440 Y2.0

• N445 Y2.5

• N450 Y3.0

• N455 Y3.5 (Tap breaks here)

• N460 Y4.0

• N465 Y4.5

• N470 Y5.0

• .

• .

• .

• N555 G80 M09

• N560 G91 G28 Z0 M19

Admittedly, it’s a simple program – having just a few holes – but it should work nicely to stress the technique. Notice that it’s pretty efficient – the R plane is 0.1 and only the Y coordinates are specified.

Say the tap breaks when tapping the hole commanded by line N455. Here’s the modified program. Again, these modifications would be done “on the fly” after replacing the broken tap. And of course, the tap remains in the hole commanded by N455:

• (3/8-16 TAP)

• N405 T08 M06

• N410 G54 G90 S400 M03 T01

• N415 G00 X2.5 Y1.0

• N420 G43 H08 Z2.0

• N425 M08

• N430 G84 R0 Z-1.0 F25.0 L0 G98

• M99 P460

• N435 Y1.5

• N440 Y2.0

• N445 Y2.5

• N450 Y3.0

• N455 Y3.5

• N460 X2.5 Y4.0 R0.1 Z-1.0 L1 G99

• N465 Y4.5

• N470 Y5.0

• .

• .

• .

• N555 G80 M09

• N560 G91 G28 Z0 M19

Once the tap is replaced and the program is modified (a good operator can modify the program in about a minute), the operator can restart the cycle. Notice that we’ve reset the initial plane in line N420 to Z2.0. This will ensure that if the tap moves over the hole with the broken tap, it will not collide with it. The tapping command in line N430 will instate the tapping cycle but the L0 will keep a hole from actually being tapped. Also, G98 ensures that the tap will retract to the initial plane (Z2.0) at this point.

The “M99 P460” tells the control to jump to line N460. Again, the operator must know which command to restart on.

In line N460, we’ve added the X (though it wasn’t necessary in this example), the R, Z, L1 (to machine a hole for each command from now on), and the G99 to reinstate the R plane as the retract position.

Once the workpiece is finished, of course, the program must be changed back to its initial state.

One last point. We’re assuming that all tapped holes are on one side of the workpiece. If you are tapping holes on several sides of a workpiece – using a rotary device of some kind – you must also confirm that the correct side of the workpiece is facing the spindle as part of the program’s modification.

Top of page