The Optional Stop newsletter
Home | More Issues | Contact Us
From our website:
Home
Products
Services
Resources
On-Line Classes
CD-Rom Courses
CNC Books
Software
CNC Jobs
CNC Schools
CNC Tips
Educator's Page
Tech Talk Forum
Back Issues

December 28, 2011

Dear Subscribers,

Welcome to Issue 89!  We at CNC Concepts, Inc. hope that you're holidays have been happy ones.  And wish you the best for 2012.

We've put together another diverse issue of The Optional Stop and hope you enjoy it.  As always, we're interested in hearing your opinions, suggestions, and comments.  If you have an idea you'd like to see published, be sure to submit it!

Again, enjoy! 

 

Mike Lynch

IN THIS ISSUE
Product Corner: ME Consultant Pro Now On Sale
Instructor Note: Explaining radius compensation
Manager's Insight: Bare minimums for CNC operators
G Code Primer: Leave yourself a life-line when changing programs
Macro Maven: A unique bolt-circle custom macro
Parameter Preference: Switching between measurement systems (Imperial and Metric)
Safety First: Be sure newcomers understand safety issues

Product Corner: ME Consultant Pro Now On Sale

This little program gem is great for helping you determine how long machining operations will take. The Machining Calculator is easy to use and automatically selects cutting conditions (speed, feedrate, etc.) from a user-definable material file. The job planner allows you to string together any number of machining operations to determine how long a completed workpiece will take to machine.

If you haven’t already checked out this great program, now is the time! We’re offering it for $20.00 off the normal price – now only $129.95.

 

M01

Top of page

Instructor Note: Explaining radius compensation

Both machining centers and turning centers have a form or radius compensation – cutter radius compensation on machining centers and tool nose radius compensation on turning centers. Either of these forms of compensation can be difficult to explain in class. Students tend to have difficulties understanding how radius compensation works and especially how to program it.

The first difficulty often has to do with understanding whether to use G41 or G42 to instate (tool left and tool right). The “standard” explanation is to say something like “Look in the direction the cutting tool is moving and ask yourself if the cutter is on the left side for right side of the surface being machined. If the cutter is on the left, you’ll use G41 to instate. If it’s on the right, you’ll use G42.”

This explanation often works, but some students may have trouble visualizing the motion in the direction the cutter is moving. Or in remembering that it is the cutter that is in question, not the work surface. So be prepared to go a bit further.

With turning centers, it can be pretty easy. Simply say that external turning (toward the chuck) is G42 and internal boring (again, toward the chuck) is G41. External facing is also G41. There’s not much more to it for lathe-work. Students can simply take it at face value that turning is G42 and boring is G41.

For machining centers a similar technique can be used, as long as students know the difference between climb milling and conventional milling. With right hand cutting tools (spindle running forward, M03), climb milling will require instating cutter radius compensation with G41. Conventional milling requires G42.

Another difficulty machining center students have is understanding how to position the cutter just before the instating command. I call this cutter location the “prior position”. Explain that it is important to position the cutter at least the maximum cutter radius size away from the first surface to be machined – and so that the instating command motion forms a right (90 degree) angle to the motion for the first surface to machine.

If this rule is broken and the cutter is less than its radius away from the first surface to mill, most controls will generate an alarm – the over-cutting alarm. The machine will think it is already violating the first surface to be milled when cutter radius compensation is instated.

Yet another difficultly for machining center people is related to what actually happens during the cutting tool’s machining motions. Be sure to point out that there is nothing magical going on. During each motion under the influence of cutter radius compensation, the machine is simply looking ahead to see the direction for the next motion in order to determine the location for the motion’s end point. It will simply keep the cutter flush with and on the left side (with G41) or right side (with G42) of all surfaces being machined.

Canceling (with G40) can also present a problem for newcomers. For turning centers, it’s simple. Just include a G40 on the tool’s retract to the turret index position. But with machining centers, it can be more difficult.
I like to have machining center people bring the cutter to a clearance position that is away from machined surfaces – if it is possible. Then, still under the influence of G41 or G42, retract the cutter in Z to a position that is clear of the workpiece. Finally, include a G40 in a command by itself. With some machines, the tool may move in X and/or Y by the amount of the cutter radius compensation offset, but that’s okay – since the tool is clear of the workpiece in Z.

If clearing the workpiece in Z is not possible, then make sure students understand that any X and/or Y motion that includes a G40 will end with the cutter’s center at the programmed X/Y position. With this understanding it is always possible to make an acceptable canceling command.

M01

Top of page

Manager's Insight: Bare minimums for CNC operators

Getting CNC people together with CNC-using companies seems to have become quite a challenge in recent years. CNC-using companies will tell you that they cannot find qualified CNC people – at least not at the wages they’re willing to pay. CNC people will tell you that they cannot find companies hiring CNC people. For this reason, more and more CNC-using companies are hiring people with limited CNC experience – even with limited shop experience – and providing on-the-job training.

Editor’s note: My web site www.cncci.com provides a free jobs page to help employers find CNC people. We provide listings for people looking for jobs as well as listings for companies looking for people. You can find more information here: http://www.cncci.com/resources/jobs.htm

From a numbers standpoint, the CNC position that commonly requires the most people in a company is that of CNC operator. For example, a single-shift company that uses ten CNC machines may have but one or two programmers, two or three setup people, but as many as seven to ten operators. This often means companies have the most difficulties when it comes to fully staffing CNC operator positions.

One common misconception about the CNC operator position – one that often contributes to the long-term staffing problem – is that a person doesn’t have to know very much about CNC or manufacturing in general in order to be a successful CNC operator. Indeed, I’ve heard more than one manager say that anyone can push buttons and load parts. While there are applications that have been engineered to a level that minimize the need for operator skills – even to the point that they require little more than button pushing – these applications are few and far between. The vast majority of CNC operator jobs require much more knowledge and skill.

Here I will list what I consider to be the bare minimums. Note that I’m limiting this discussion to the CNC operator position. That is, the person who completes the production run. Someone else programs the job and sets it up. During the setup, the first workpiece is run and has passed inspection. Maybe a few more parts are run to ensure that the process is stable. At this point, the CNC operator takes over and runs the rest of the workpieces.

CNC operator responsibilities commonly include loading and unloading workpieces, activating and monitoring the cycle, cleaning completed workpieces, measuring completed workpieces, determining when a critical workpiece attribute is getting close to a tolerance limit, making sizing adjustments to ensure that subsequent workpieces are acceptable, reporting to a statistical process control (SPC) system, determining when cutting tools are getting dull, and replacing worn cutting tools.

Some companies expect even more. They may expect the operator to, among other things, run multiple machines – possibly dissimilar machines – perform secondary operations on completed workpieces, and perform certain preventive maintenance tasks (like cleaning and maintaining lubricant levels).

Obviously, the more you expect, the more your operators need to know. Again, here are what I consider to be the bare minimums.

Shop safety – Your operators must recognize the potential for dangerous situations and be able to use safe shop practices. They must know how to handle themselves around the shop in general and they must know the specific dangers and safety practices related to the machine/s they run.

General machine usage – The operator must understand enough about the machine to be able to activate needed functions. Ideally, they should understand the purpose of every button and switch on the machine – even if they don’t have need of it. But at the very least, they must understand those functions they will regularly use as well as master the various procedures needed to run the machine. These procedures include (among others) power up, workpiece loading, cycle activation, offset adjustment, manual tool changing, manual movement (jog and handwheel), and shut-down.

Shop math – The math required of CNC operators is pretty simple – mostly adding and subtracting. The trick is being able to perform simple arithmetic calculations – over and over again – without making any mistakes.

Blueprint reading – Since the CNC operator will always have a completed workpiece to reference (made by the setup person), interpreting the blueprint will be easier than it would otherwise be. But the CNC operator must still be able to recognize specifications on the blueprint for the various surfaces being machined – especially for critical surfaces.

Tolerance interpretation – The blueprint, of course, specifies a tolerance for every machined surface. A CNC operator must be able to determine each tolerance, as well as whether each machined surface is acceptable or not. They must be able to calculate high and low limits for every tolerance, and determine when a surface is growing or shrinking (due to tool wear) to a point that it is coming close to a tolerance limit. When a surface is getting close to a tolerance limit, they must be able to determine the deviation amount and direction. That is, the difference between the measured value and the target value for the surface as well as the polarity (plus or minus) for the needed adjustment. Finally, they must know how make the adjustment (commonly with an offset) so that the surface will be machined at its target value for subsequent workpieces.

Measuring devices – Your CNC operators will probably be using a variety of measuring tools in order to measure workpiece attributes. At the very least, they will probably be using variable gages like micrometers and calipers. Mastering variable gages takes practice and skill. They must, of course, be able to properly use the gages you provide.

Cutting tools – If you expect your operators to replace worn tools, they must be able to recognize when tools are getting dull and have the skills to replace them. They must be able to remove them from the machine and use the hand tools required to replace the cutting part of the tool. If they change the cutting tool’s condition (length, diameter, etc.), they must also be able to measure the cutting tool attribute and enter the appropriate value into an offset. If the cutting tool must perform a critical machining operation, they must also be able to use trial machining techniques (as the setup person does when machining the first workpiece) to ensure that the next machined workpiece is a good one.

You may be able to come up with more essentials for your CNC operators (and I’d love to hear them). Though CNC operators are often the least paid people in CNC using companies, they are among the most important. When you think about it, they may be the only ones that actually make your company any money – since it is only when machines are running production that your products are getting closer to completion. As a manager, it’s up to you to ensure that they’re getting what they need in the way of training in order to function at peak levels.

M01

Top of page

G Code Primer: Leave yourself a life-line when changing programs

 by Doug Rinehart

Every programmer-operator has to make changes to a program from time to time “on the fly” during-a parts run. It is quite easy to lose your train of thought during such changes, which opens the door to making mistakes – especially if you don’t have a hard copy of the program. I recommend using a technique developed while changing parameters: document the current setting before making changes. With this technique, you’re throwing yourself a kind of “life-line” that gives you the ability to change the program back to its original state if you need to.

This technique is especially helpful when you are "just trying different things" or editing the program while "tweaking", correcting that crucial dimension.

You can use parentheses to leave the life-line. This way you don’t have to write anything down, and documentation will remain in the program for all to see at some future date.

Example: you need to try a different value for a positioning move, so document the old amount.

  • G01 X4. Y4.01 (Y4.005) F20.0

By putting the old amount in your lifeline, you can easily refer to it or trace back to what you had previously used. You could even include a note specifying why you made the change.

M01

Top of page

Macro Maven: A unique bolt-circle custom macro

by Tom Sorrentino of Nazareth Machine Works

If a tool breaks or dulls during a CNC cycle, the operator must replace the tool and restart the program from the last hole machined. This custom macro allows the ability to do just that: start and finish with any hole on the bolt circle. The more holes there are on the bolt-circle, the more useful this program will be.

We simply provide the custom macro and example calling programs here – so you can easily copy and past them into your own text editor. Click the link below to get instructions (a .pdf file).

One point that is not explained in the instructions is that permanent common variable #501 is used as the hole counter, meaning should a tool break, the operator can view this variable to determine where the custom macro left off. This keeps them from having to count holes.

  • O1001 (BOLT HOLE MACRO

  • (---INPUT-CHECKS---)

  • #19=[FIX[ABS[#19]]] (GET POSITIVE INTEGER, REGARDLESS OF INPUT)

  • IF [#8EQ0] THEN #11=[FIX[ABS[#11]]] (ROUNDS H AS INTERGER FOR EQ. SPACED B.C.)

  • #18=ABS[#18]

  • #3=[FIX[ABS[#3]]]

  • #9=ABS[#9]

  • IF[#19EQ#0] THEN #19=1

  • IF[#19LE0] THEN #19=1

  • #8=ABS[#8]

  • IF[#8EQ#0] THEN #8=#11

  • IF[#8EQ0] THEN #8=#11

  • IF[#8GT#11] THEN #8=#11

  • (---ERROR-CHECKS-&-MESSAGES---)

  • IF[#11EQ#0] THEN #3000=101(H-NOT-DEFINED)

  • IF[#11EQ0] THEN #3000=101(H-NOT-DEFINED)

  • IF[#19GT#11] THEN #3000=102(S-OUT-OF-RANGE)

  • IF[#24EQ#0] THEN #3000=103(X-NOT-DEFINED)

  • IF[#25EQ#0] THEN #3000=104(Y-NOT-DEFINED)

  • IF[#26EQ#0] THEN #3000=105(Z-NOT-DEFINED)

  • IF[#18EQ#0] THEN #3000=106(R-NOT-DEFINED)

  • IF[#18EQ0] THEN #3000=106(R-NOT-DEFINED)

  • IF[#7EQ#0] THEN #3000=107(D-NOT-DEFINED)

  • IF[#1EQ#0] THEN #3000=108(A-NOT-DEFINED)

  • IF[#3EQ#0] THEN #3000=109(C-NOT-DEFINED)

  • IF [[#3LT73]OR[#3GE89]] THEN #3000=110 (C-OUT-OF-RANGE)

  • IF[#17EQ#0] THEN #3000=111(Q-NOT-DEFINED)

  • (---CALCS-&-MOV'T---)

  • N1 #501=#19 (INITIALIZE COUNTER)

  • #102=[360/#11] (ANGLE BETWEEN HOLES)

  • #103=[#1+[#102*[#19-1]]] (INITIALIZE CURRENT ANGLE)

  • #104=[#26+0.1] (RAPID APPROACH PLANE)

  • #105=[#26-#7] (Z BOTTOM OF HOLE)

  • #11=#8

  • IF [#3EQ74] THEN M5 (SPINDLE STOP)

  • IF [#3EQ74] THEN M4 (SPINDLE REVERSE)

  • IF [[#3EQ74]OR[#3EQ84]] THEN M29 S#4119 (RIGID TAPPING)

  • MATCHES CURRENT SPINDLE SPEED)

  • N2 IF [#501 GT #11] GOTO 99 (TEST IF LOOP IS FINISHED)

  • #110=[#24+COS[#103]*#18] (CALC X POS FOR CURRENT

  • HOLE BASED ON CURRENT ANGLE)

  • #111=[#25+SIN[#103]*#18] (CALC Y POS FOR CURRENT HOLE BASED ON CURRENT ANGLE)

  • G98 G#3 X#110 Y#111 R#104 Q#17 P#20 Z#105 F#9 (MACHINE CURRENT HOLE

  • G80 (CANCEL CYCLE)

  • #501=[#501+1] (STEP COUNTER)

  • #103=[#102+#103] (STEP CURRENT ANGLE)

  • GOTO 2 (LOOP RESTART)

  • GOTO99

  • N3 (---NOTES---)

  • (MUST ENTER ALL INFO COMPLETE)

  • (X - POSITION X TO CENTER OF BOLT HOLE PATTERN)

  • (Y - POSITION Y TO CENTER OF BOLT HOLE PATTERN)

  • (Z - SURFACE IN Z WHERE HOLES ARE LOCATED)

  • (R - RADIUS OF THE BOLT HOLE PATTERN)

  • (D - DEPTH OF HOLES)

  • (A - START ANGLE, 0 IS THREE O'CLOCK, PLUS IS CCW)

  • (H - NUMBER OF HOLES)

  • (C - CYCLE TYPE, 81 IS DRILLING, 84 TAPPING, ETC.)

  • (Q - PECK VALUE)

  • (F - FEEDRATE)

  • (S - START HOLE NUMBER, USED TO RESUME AFTER TOOL BREAKAGE)

  • (E - END HOLE NUMBER, USED WHEN DOING HOLES ON AN ARC)

  • (T - MS DWELL VALUE WHEN NEEDED)

  • (SET S=1 & E=0 FOR ALL HOLES MACHINED)

  • (G74 & G84, FEED & SPINDLE SPEED MUST BE MATCHED TO LEAD OF TAP USED)

  • (MODIFIED ORIGINAL FROM CNC COCEPTS, INC.)

  • (TOM SORRENTINO, NAZARETH MACHINE WORKS)

  • (USE AT OWN RISK, PROVE OUT BEFORE MACHINING)

  • N99 (END)

  • M99

M01

 

Top of page

Parameter Preference: Switching between measurement systems (Imperial and Metric)

Admittedly, most companies work exclusively in one measurement system mode or the other (inch or Metric). If they happen across a print dimensioned with the other measurement system, it is converted to and run in the preferred measurement system. If this is the case, it really doesn’t matter what happens when measurement system modes are changed (the company never changes from one to the other).

There are some companies, however, that have the need to use both measurement system mode. Possibly they have an equal number of jobs dimensioned in each measurement system. Or they may be trying to gain a resolution advantage by running workpieces dimensioned in the Imperial system in the Metric mode. Regardless of the reason, it is important to know that a parameter controls what happens to certain values (like axis positions and offset data) when you switch measurement system modes.

Either the decimal point will simply move one place to the left or right or a true conversion will take place. Here is an example of each.

If the decimal point simply moves, an X axis position display of 10.0000 (inches) in the Imperial system will be shown as X100.000 when the Metric mode is selected. Ten inches, of course, is not equal to one-hundred millimeters.

If a true conversion takes place, an X axis position display of 10.0000 (inches) in the Imperial system will be shown as X254.000 when the Metric mode is select.

A reciprocal conversion is done, of course, when the inch mode is reselected.

As you may have guessed, many machines have a parameter that controls what happens when measurement system modes are changed. As with all parameters, the parameter number varies among the various control models. You can find documentation about this parameter in the measurement system selection descriptions (usually with G20 and G21) in the Fanuc Operator’s manual.

M01Top of page

Safety First: Be sure newcomers understand safety issues

It’s refreshing to say that we’re beginning to see a upturn in manufacturing – at least in some sectors and parts of the country. With the increase in work comes the need for new people. Unfortunately, some companies are finding it difficult to find people with shop experience, let alone CNC experience. For this reason, they must hire people with little or no previous experience in a shop environment and training them from scratch.

One of the first issues you must deal with is safety. Remember that safety practices you take for granted – or feel are common sense – are unknown to people that have never been in a machine shop. It’s likely that any previous working conditions they have experienced include no safety-related issues. That is, the idea that something in their work environment could be dangerous may be a new concept for them.

Be sure that initial training topics – or their orientation to your company – include safety issues. Begin by explaining general safety practices – like the proper use of safety equipment (safety glasses, gloves, etc.), how to avoid hazards when moving from place to place in the shop (staying within yellow lines, never taking short-cuts, avoidance of vehicles, and use of mirrors), and the meaning of all safety signs.

Be sure they understand, of course, more specific safety issues related to the tasks they will be assigned. And again, don’t assume anything.

M01

Top of page

 
 
Sofware ad
 
Machining center training materials
 
Parametric programming ad

The Optional Stop newsletter is published quarterly by CNC Concepts, Inc. and is distributed free of charge to people subscribing to our (email) distribution list and to those downloading it from our website (www.cncci.com). Information is aimed at CNC users and instructors teaching live CNC classes. All techniques given in this newsletter are intended to help CNC people. However, CNC Concepts, Inc. can accept no responsibility for the use or misuse of the techniques given.

To subscribe: Simply email us (newsletter@cncci.com) and let us know you'd like to be added to our distribution list.

To unsubscribe: Respond to this email, typing REMOVE in the subject. Please accept our apologies if we have disturbed you.

ThirtyThirty hotel
Powered by Best Free Counters