OverviewDuring the past decade, Peter Smid wrote dozens of column
for Shop Talkmagazine that addressed the full gamut of CNC
topics, such as tapping and threading and knurling; program length
and memory needs; G-codes, M-functions, cycles, macros … and more
still. Ever since Shop Talk ceased publication,
these columns have been unavailable. Now, in CNC Tips and
Techniques, we are delighted to bring them back—over 60 of the
best of Peter’s columns --- all under one cover, so that you can
have full and easy access to the advice Peter has been sharing
during the past decade. CNC Tips and Techniques is a treasure
trove of Peter Smid’s “lost work” that is certain to be an
invaluable addition to your CNC toolkit. We hope the advice
and instructions contained in these readings will help you do your
job more efficiently and more effectively – and that you find
them a good read besides. Features Offers more than 60
focused columns which have been thoroughly reviewed since its
initial publication and updated as needed to reflect ongoing
changes in the field. Columns are presented here in chronological
order of when they first appeared. Includes an alternative table of
contents, organized by topic. Provides several useful appendices
and an extensive index. Appeals to both veterans and newcomers with
tips and techniques that can be applied at work and speed up the
learning curve. Peter Smid is a professional consultant,
educator and speaker, with many years of practical, hands-on
experience, in the industrial and educational fields. During his
career, he has gathered an extensive experience with CNC and
CAD/CAM applications on all levels. He consults to manufacturing
industry and educational institutions on practical use of
Computerized Numerical Control technology, part programming,
Autocad®, Mastercam® and other CAD/CAM software, as well as
advanced machining, tooling, setup, and many other related fields.
His comprehensive industrial background in CNC programming,
machining and company-oriented training has assisted several
hundred companies to benefit from his wide-ranging
knowledge. Mr. Smid’s long time association with
advanced manufacturing companies and CNC machinery vendors, as well
as his affiliation with a number of Community and Technical College
industrial technology programs and machine shop skills training,
have enabled him to broaden his professional and consulting skills
in the areas of CNC and CAD/CAM training, computer applications and
needs analysis, software evaluation, system benchmarking,
programming, hardware selection, software customizing, and
operations management. Over the years, Mr. Smid has developed and
delivered hundreds of customized educational programs to thousands
of instructors and students at colleges and universities across
United States, Canada and Europe, as well as to a large number of
manufacturing companies and private sector organizations and
individuals. He has actively participated in many industrial trade
shows, conferences, workshops and various seminars, including
submission of papers, delivering presentations and a number of
speaking engagements to professional organizations. He is also the
author of articles and many in-house publications on the subject of
CNC and CAD/CAM. For six years he had a monthly column in the
ShopTalk Magazine related to CNC programming. During his many years
as a highly respected professional in the CNC industrial and
educational field, he has developed tens of thousands of pages of
high quality training materials. The author welcomes comments,
suggestions and other input from educators, students and industrial
users. You may contact him at
[email protected]. Also by
Peter Smid: CNC PROGRAMMING TECHNIQUES An Insider's Guide to
Effective Methods and Applications FANUC CNC CUSTOM MACROS
Practical Resources for Fanuc Custom Macro B Users Sample
Readings Programming a Long Thread Trial Cut
for Measuring Special-Purpose G-Codes Running the
First Part — Economically, That Is Programming a
Long Thread 1. Programming a Long Thread
In the essay Limitations in Threading, the main focus was on
limitations in single point threading caused by spindle speed that
is either too high or too low. In this essay, we look at the effect
of threading feedrate, particularly how it applies to long threads.
What exactly is a long thread may be a subject for some
discussion. For the purposes of this article, a long thread is a
thread with a ratio of rather small diameter to long threading
length. In most everyday threading operations, you will work with
threads that have a length relatively short respective to their
diameter. These threads, which do not require any physical support
at the machine, generally do not present any problems in
programming or machining. Machining long threads does have a few
challenges, however. Long threads often require suitable support
devices, at least a tailstock for basic support, but often a
follower rest or a steady rest as well, in order to prevent
deflection of the part. Many CNC machine tool builders
provide lathes specially designed for machining long parts, such as
shafts and tubular stock. These lathes (often of the flat bed type)
are also capable of threading over their entire Z-axis
travel. From the CNC programmer's perspective, a possible problem
lies with the feedrate for certain imperial threads.
Feedrate for threading is always the thread lead, and no rounding
is necessary for metric threads. Some imperial threads have to use
rounding for feedrate calculation, when the threads per inch (TPI)
are converted to the thread lead (cutting feedrate). As an
example of a possible problem of feedrate rounding, consider a
single start, standard form 60 degree thread 6.0-12, over the
threading length of 70 inches (actual use of the thread is not
important for the illustration): Thread diameter = 6.0
inches Thread per inch (TPI) = 12 Length of thread = 70 inches
Assuming a suitable tooling and part setup, the thread
cutting program is easy: N51 T0500 N52 G97 S550 M03
(SPINDLE SPEED 550 RPM) N53 G00 X6.25 Z0.4 T0505 M08 (START
POINT CLEARANCE) N54 G76 P011060 Q005 R0.002 (G76 - BLOCK 1)
N55 G76 X5.8978 Z-70.0 R0 P0511 Q0120 F0.0833 (G76 - BLOCK 2
- 0.0833 IPR) N56 G00 X12.0 Z5.0 T0500 (TOOL CHANGE
CLEARANCE) N57 M01 All program data look reasonable, but let's
focus on the programmed feedrate of F0.0833. For twelve threads per
inch, the pitch is 1/12 = 0.08333333, which is also the thread lead
and programmed feedrate. Now, consider the feedrate actually used
in the program, F0.0833. It has been rounded to four decimal
places, as is customary for imperial dimensions. Inevitably, the
rounding has brought in a certain amount of inaccuracy. Over one
inch length, the error is: 1 - 12 * 0.0833 = 0.0004 inches In most
cases, this error can be absorbed by the thread tolerances. Now,
consider the same error over a significant thread length, such as
our example of 70 inches: 70 * 0.0004 = 0.0280 inches —
this is a significant error Because the 0.0833 amount was the
correct rounding to four decimal places, any other rounding would
make the accumulative error even worse. The solution to this
problem is quite simple — just change the programmed feedrate
of F0.0833to a new feedrate of F0.083333, from four to
six decimal places. Fanuc-type controls allow this method, for the
exact purpose of minimizing the accumulative error for long
threads. With F0.083333, the error over 70 inches will be: 1
- 12 * 0.083333 = 0.000004 inches * 70 = 0.00028, which is less
than three tenths. Older Fanuc and similar controls could not use
F-addresses with six decimal places, but the control provided
E-addresses, specifically for threading, which did allow six
decimal places. The six decimal place accuracy is not required for
threads that have lead divisible into four or fewer decimal places,
for example 16 TPI = 1/16 = 0.062500. The G76 threading cycle
itself will be discussed in two other essays looking at basics and
details. 2. Trial Cut for
MeasuringPrecision CNC machining is always a cooperative effort
between CNC programmers and CNC machine operators. Programmers can
employ certain program features that will enable the machine
operators to perform functions that would otherwise be difficult or
even impossible. One such method is programming a trial cut
for measuring. There are many factors in machining that influence
the final size of a part, such as heat, tool deflection, tool wear,
and even lubrication to some extent. For those parts that require
very tight tolerances, the negative effect of these factors may
result in an out of tolerance size and even a possible scrap.
Another problem that is quite common is machining certain
hard-to-measure shapes, such as a cone on CNC lathes. By using a
simple programming method known as the trial cut, CNC
programmers can greatly influence the final size of a part. Take
the already mentioned cone as an example. Without a suitable custom
gauge, a cone is a difficult shape to measure at the machine, as
there is no flat spot for the micrometer to use. Even if such a
special gauge is available, it will be too late to find out that
the cone is out of tolerance. The method of using a trial cut is to
provide a special flat area (diameter) that can be easily measured,
before the final cone is machined, following a few simple rules.
Normally, a cone machined from round stock, such as the 5.0 inch
diameter used in the following example, will include G71 roughing
cycle and G70 finishing cycle in the part program: N1 G20 T0100
(ROUGHING TOOL) N2 G96 S300 M03 (CUTTING SPEED) N3 G42 G00 X5.2
Z0.1 T0101 M08 (START POINT FOR CYCLE) N4 G71 U0.15 R0.025 N5 G71
P6 Q8 U0.07 W0.02 F0.015 N6 G00 X2.8 (CONE START) N7 G01 X4.6 Z-3.5
F0.008 (CONE END) N8 U0.2 (RETRACT FROM PART) N9 G40 G00 X10.0 Z4.0
T0100 (CLEAR POSITION) N10 M01 N11 T0300 (FINISHING TOOL) N12 G96
S500 M03 (CUTTING SPEED) N13 G42 G00 X5.2 Z0.1 T0303 M08 (START
POINT FOR CYCLE) N14 G70 P6 Q8 N15 G40 G00 X10.0 Z4.0 T0300 (CLEAR
POSITION) N16 M30 % Although correct, the program above does not
offer any means to measure the conical part efficiently. By adding
several blocks of trial cut in the program and using the finishing
tool (T03), a suitable straight cut can be machined first. When
measured, various offsets can be adjusted as necessary — all this
is done before any roughing cuts take place: / N1 G20 T0300
(FINISHING TOOL) / N2 G96 S500 M03 (CUTTING SPEED) / N3 G42 G00
X5.2 Z0.1 T0303 M08 (INITIAL POSITION) / N4 X4.925 (DIAMETER TO BE
MEASURED) / N5 G01 Z-0.35 F0.008 (LENGTH OF CUT FOR MEASURING) / N6
U0.2 (RETRACT) / N7 G40 G00 X10.0 Z4.0 T0300 (CLEAR POSITION) / N8
M00 (MEASURE DIAMETER - MUST BE 4.925) N9 G20 T0100 (ROUGHING TOOL)
N10 G96 S300 M03 (CUTTING SPEED) N11 G42 G00 X5.2 Z0.1 T0101 M08
(START POINT FOR CYCLE) N12 G71 U0.15 R0.025 N13 G71 P14 Q16 U0.07
W0.02 F0.015 N14 G00 X2.8 (CONE START) N15 G01 X4.6 Z-3.5 F0.008
(CONE END) N16 U0.2 (RETRACT FROM PART) N17 G40 G00 X10.0 Z4.0
T0100 (CLEAR POSITION) N18 M01 N19 T0300 (FINISHING TOOL) N20 G96
S500 M03 N21 G42 G00 X5.2 Z0.1 T0303 M08 (START POINT FOR CYCLE)
N22 G70 P14 Q16 N23 G40 G00 X10.0 Z4.0 T0300 (CLEAR POSITION) N24
M30 % The first eight blocks are shown with a block skip function,
represented by the / symbol. It is more likely that the actual
measuring will not be required for each part. This approach to part
programming is more efficient because it eliminates a re-cut and
greatly enhances accuracy. Setting the block skip mode OFF, CNC
operator checks the trial dimension (note the message attached to
M00 program stop function), adjusts the suitable offset if
necessary, and continues machining with block skip set ON. Note
that the trial cut was done with the same tool that will be used
for finishing. When selecting trial cut diameter, make sure the
tool removes about the same amount of material that is removed in
the finishing cut. In the example, the trial cut diameter is 4.925,
resulting in the actual depth of cut (5.0 – 4.925) / 2 = 0.0375
per side, which is almost equivalent to the amount of stock left
for finishing: 0.07 / 2 = 0.035 per side. The length of such
a cut should be sufficient for micrometer (0.35 in the
example). Also, the machining speed and cutting feed rate
should be the same for best results. The trial cut is a special cut
performed on demand only. Although a lathe example has been
presented here, trial cuts have many applications in milling
operations as well. The main key is to identify the need first;
then, provide a suitable program.
3. Special Purpose G-CodesAnybody even
loosely associated with CNC work is probably familiar with the
G-codes, at least with their existence. Preparatory commands,
as they are officially called, have a single purpose — they give
a specific meaning to other commands in the part program. For
example, a programmed command X10.0 can be interpreted as 10 mm, 10
inches, or even as 10 seconds. If this command represents a
dimensional program entry, it could be an absolute position or an
incremental distance and direction, in rapid or feedrate mode. The
exact meaning is defined by one or more G-codes. For example, an
incremental feedrate motion of 10 mm will require that G21 (metric
mode), G91 (incremental motion), and G01 (linear interpolation)
commands are in effect, along with appropriate feedrate.
Many preparatory commands are well known to CNC programmers
and operators alike, as they are used in virtually every program,
such as those shown in the example. Yet, a list of G-codes for a
particular control can be quite long and contain many that are
hardly used. Typically, a preparatory command will have two digits
following the letter G. Three digit G-codes generally identify the
G-code as a particular cycle or function to the CNC machine that
uses them; they are not usable anywhere else. Three-digit G-codes
are often special macros supplied by a particular machine tool
builder. Within the two-digit category of G-codes, there are also
several that are fairly common, yet hardly ever used in a part
program. One pair is G22/G23, defined as Stored
Stroke Check, ON and OFF respectively. In plain terminology, using
these commands allows the programmer to define special
three-dimensional zones either as ones that allow a tool from
entering or as zones that prohibit a tool from entering. Such
definitions may prevent a collision with a certain part of the
machine or a fixture. A relatively recent pair of other
G-codes, G25/G26, is used to detect severe spindle
fluctuation caused by heat. When G26 Spindle Fluctuation
ON is in effect, the control system monitors whether the
fluctuation is within specified tolerance range or not. Should the
tolerance be exceeded, the control will issue an alarm, warning the
user. In order to use this function correctly, a consultation with
a service technician is recommended. Another set of G-codes
is a foursome related to the return to machine
zero: G27/G28/G29/G30. Whereas the G28 command and, to a
large extent, the G30 command are used to move the specified axis
or axes to the machine zero (G28 to the primary and G30 to the
secondary machine zero), the G27 and G29 are seldom, if ever, used
in a typical part program. Command G27 is a machine zero
position check. It is programmed with one or more axes and checks
whether the position specified corresponds to machine zero
position. If not, the program processing stops and alarm is raised
by the control. Its practical application has ceased with the
demise of G92 (G50) programming (position register). There is
no need for this command in a program that uses work offsets (G54
to G59 or higher). G29 is the opposite of G28/G30. Whereas G28/G30
represents a motion to machine zero via an intermediate point, G29
is a motion from machine zero to a specified position via an
intermediate point. This command is virtually useless in typical
programs. Another virtually useless command
is G44 (tool length offset negative). It may have its
adherents, but there is nothing that the ubiquitous G43 command
(tool length offset positive) cannot achieve. A command that
may be somewhat of a puzzle is G31, defined simply as
the Skip command. This command is indeed a very special one
because it is exclusively used with probing on CNC machines
(in-process gauging). Its purpose is to move the probe from a clear
position, at a feedrate (just like G01), to a position to be
probed. Once the probe detects a contact with the material, the
motion stops and the remainder of the motion is not completed; it
is skipped, hence the command name. Finally, there are
several G-codes in the G6x range, namely G60 (Single
direction positioning), G61 (Exact stop check
mode), G62 (Automatic corner override
mode), G63 (Tapping mode), and G64 (Normal
cutting mode). The default is G64, normal cutting mode. G61
is the modal version of G09, and can be useful for increased
precision when a tool has to move around a sharp corner at a high
feedrate, particularly if the corner forms a narrow angle. G62 may
improve the surface finish when used to cut sharp inner corners in
cutter radius offset mode. Its function is to automatically adjust
the cutting feedrate. A tapping mode programmed with G63 disables
the feedrate override and the feedhold button, and G64 returns the
cutting motions to their original programmed mode. Each mode
selected replaces any other mode. G60 stands
separately. Its purpose is to force a unidirectional tool
positioning, regardless of which direction the tool comes from. It
can be used to compensate for some minor backlash, but it
does not remove it. Backlash problems require qualified
service technicians. There may be other G-codes not commonly
used, but the ones mentioned in this column should provide some
understanding of the more common special purpose G-codes.
4. Running the First Part —
Economically, That IsMachining a batch of the same parts in a
single production run is probably the most common reason for
purchasing a CNC machine. The CNC technology offers a great amount
of predictability. There is consistency between parts, dimensional
accuracy is maintained over many parts, and the program and setup
— once verified — can be used over and over in the future. Yet,
even with proven part programs, the production always hits one weak
spot when running a new batch. Yes, it is the first part.
Every supervisor knows that the first part of the batch is also
the most expensive part of the whole batch; its cost of
manufacturing proportionally affects all remaining parts. To
minimize the cost of making the first part, it is worth looking at
several influencing factors and possible solutions. Comparing
Programs There is a significant difference between running the
first part using a new program and a program that had already been
verified. New part programs CNC programs that have never been used
must be carefully inspected. Even programs generated by a CAD/CAM
system require certain scrutiny, although on a much smaller scale.
Programming errors and oversights can find their way into any
program in various forms, some quite hard to detect. For example,
the depth and width of a cut may be out of a reasonable range,
clearances may be too large or too small, spindle speeds and feed
rates may be overrated or underrated, a tool may not be the most
suitable one for the job, and so on. These oversights are virtually
impossible to see in print or even on the screen — they show only
when the first part is run on the CNC machine. In addition to the
program itself, the machine setup is always new, regardless of
whether the program is new or previously verified. Verified part
programs These are part programs accepted for production and
verified at some earlier date. Keep in mind that only the programs
have been verified, not the setups or tools. Setups and tools are
subjects to frequent changes; they must be verified every time.
Another important consideration is the CNC machine tool being used.
Even verified programs have to be checked if they are used on a
different machine than the previous time. Decreasing Costs
Decreasing the cost of the first part — and, therefore, the whole
batch — has to be considered at four levels, all interrelated:
Planning Process planners or supervisors have to evaluate many
aspects of the production. One of their key considerations is the
number of parts produced in a single batch. The more batches per
period of time, the more expensive each batch will be, mainly
because of the repeated setups. Assuming that more parts produced
in a batch will have no negative side effects (for example, on
inventory), fewer batches per period of time might provide part of
the solution. 5. Programming CNC
programmers can literally do wonders to decrease the cost of the
first part through the program. Here are only some ideas. Using
consistent tool numbers for commonly used tools saves time during
setup, as tool registration and many related offsets will not
change. Another very effective programming method is to include one
or more trial cuts with the block skip function in the program.
These cuts will only be used for the first part testing, but turned
off for a full run (except the occasional inspection). Don't forget
to provide sufficient comments in the program, so the operator
knows the purpose of these special cuts. Another consideration,
especially for programs developed manually, is to invest in
reliable CNC simulation software. Although no software can simulate
every detail of CNC machining, it can be an excellent tool to find
errors and areas of improvement. Setup At the machine, the CNC
operator is normally responsible for setting up tools and fixtures,
registering tool numbers and various offsets, troubleshooting the
program, and monitoring the operation. Speeding up the
non-productive time required for setup is the most significant
single saving available. Modular fixturing, common tooling, general
setup consistency, and the operator's skill all add up to make the
transition between setup and operation faster and smoother.
Machining During machining, the CNC operator relies heavily on the
program itself. During the first part run, it should not be enough
for the CNC operator to look just for errors or monitor the program
flow. Operators can and should do much more at the same time. For
example, they can think about optimizing the program for better
performance. Speeds and feeds are the most common areas to focus
on, but many more “little things” also influence the cost of
manufacturing (including the first part). Lowering the cost of the
first part should be a team effort. CNC programmers may be the key
people in such efforts. However, mutual cooperation of everybody
involved will offer many benefits and have a positive effect on the
proverbial bottom line. OPERATIONS General Cutting
Knurling Lathes Machines Tapping Threading Tools
Turning PROGRAMMING Programming Techniques
Subprograms Toolpaths CODES, FUNCTIONS, AND MACROS
Codes Functions Macros CYCLES THE MATHEMATICS OF
CNC CNC GEOMETRY WORKING IN THE FIELD
Welcome to Loot.co.za!
Sign in / Register |Wishlists & Gift Vouchers |Help | Advanced search
