While the specific intention and application for CNC machines vary from one
machine type to another, all forms of CNC have common benefits. Though the
thrust of this presentation is to teach you CNC usage, it helps to understand
why these sophisticated machines have become so popular. Here are but a few of
the more important benefits offered by CNC equipment.
The first benefit offered by all forms of CNC machine tools is improved
automation. The operator intervention related to producing workpieces can be
reduced or eliminated. Many CNC machines can run unattended during their entire
machining cycle, freeing the operator to do other tasks. This gives the CNC
user several side benefits including reduced operator fatigue, fewer mistakes
caused by human error, and consistent and predictable machining time for each
workpiece. Since the machine will be running under program control, the skill
level required of the CNC operator (related to basic machining practice) is
also reduced as compared to a machinist producing workpieces with conventional
The second major benefit of CNC technology is consistent and accurate
workpieces. Today's CNC machines boast almost unbelievable accuracy and
repeatability specifications. This means that once a program is verified, two,
ten, or one thousand identical workpieces can be easily produced with precision
A third benefit offered by most forms of CNC machine tools is flexibility.
Since these machines are run from programs, running a different workpiece is
almost as easy as loading a different program. Once a program has been verified
and executed for one production run, it can be easily recalled the next time
the workpiece is to be run. This leads to yet another benefit, fast
change-overs. Since these machines are very easy to setup and run, and since
programs can be easily loaded, they allow very short setup time. This is
imperative with today's Just-In-Time product requirements.
Motion control - the heart of CNC
The most basic function of any CNC machine is automatic, precise, and
consistent motion control. Rather than applying completely mechanical devices
to cause motion as is required on most conventional machine tools, CNC machines
allow motion control in a revolutionary manner. All forms of CNC equipment have
two or more directions of motion, called axes. These axes can be precisely and
automatically positioned along their lengths of travel. The two most common
axis types are linear (driven along a straight path) and rotary (driven along a
Instead of causing motion by turning cranks and handwheels as is required on
conventional machine tools, CNC machines allow motions to be commanded through
programmed commands. Generally speaking, the motion type (rapid, linear, and
circular), the axes to move, the amount of motion and the motion rate
(feedrate) are programmable with almost all CNC machine tools.
Accurate positioning is accomplished by the operator counting the number of
revolutions made on the handwheel plus the graduations on the dial. The drive
motor is rotated a corresponding amount, which in turn drives the ball screw,
causing linear motion of the axis. A feedback device confirms that the proper
amount of ball screw revolutions have occurred.
A CNC command executed within the control (commonly through a program) tells
the drive motor to rotate a precise number of times. The rotation of the drive
motor in turn rotates the ball screw. And the ball screw causes drives the
linear axis. A feedback device at the opposite end of the ball screw allows the
control to confirm that the commanded number of rotations has taken place.
Though a rather crude analogy, the same basic linear motion can be found on
a common table vise. As you rotate the vise crank, you rotate a lead screw
that, in turn, drives the movable jaw on the vise. By comparison, a linear axis
on a CNC machine tool is extremely precise. The number of revolutions of the
axis drive motor precisely controls the amount of linear motion along the axis.
How axis motion is commanded - understanding coordinate systems It would be
infeasible for the CNC user to cause axis motion by trying to tell each axis
drive motor how many times to rotate in order to command a given linear motion
amount. (This would be like having to figure out how many turns of the handle
on a table vise will cause the movable jaw to move exactly one inch!) Instead,
all CNC controls allow axis motion to be commanded in a much simpler and more
logical way by utilizing some form of coordinate system. The two most popular
coordinate systems used with CNC machines are the rectangular coordinate system
and the polar coordinate system. By far, the most popular of these two is the
rectangular coordinate system, and we'll use it for all discussions made during
One very common application for the rectangular coordinate system is
graphing. Almost everyone has had to make or interpret a graph. Since the need
to utilize graphs is so commonplace, and since it closely resembles what is
required to cause axis motion on a CNC machine, let's review the basics of
As with any two dimensional graph, this graph has two base lines. Each base
line is used to represent something. What the base line represents is broken
into increments. Also, each base line has limits. In our productivity example,
the horizontal base line is being used to represent time. For this base line,
the time increment is in months. Remember this base line has limits - it starts
at January and end with December. The vertical base line is representing
productivity. Productivity is broken into ten percent increments and starts at
zero percent productivity and ends with one hundred percent productivity.
The person making the graph would look up the company's productivity for
January of last year and at the productivity position on the graph for January,
a point is plotted. This would then be repeated for February, March, and each
month of the year. Once all points are plotted, a line or curve can be drawn
through each of the points to make it more clear as to how the company did last
Let's take what we now know about graphs and relate it to CNC axis motion.
Instead of plotting theoretical points to represent conceptual ideas, the CNC
programmer is going to be plotting physical end points for axis motions. Each
linear axis of the machine tool can be thought of as like a base line of the
graph. Like graph base lines, axes are broken into increments. But instead of
being broken into increments of conceptual ideas like time and productivity,
each linear axis of a CNC machine's rectangular coordinate system is broken
into increments of measurement. In the inch mode, the smallest increment is
usually 0.0001 inch. In the metric mode, the smallest increment is 0.001
millimeter. (By the way, for rotary axes the increment is 0.001 degrees.)
Just like the graph, each axis within the CNC machine's coordinate system
must start somewhere. With the graph, the horizontal baseline started at
January and the vertical base line started at zero percent productivity. This
place where the vertical and horizontal base lines come together is called the
origin point of the graph. For CNC purposes, this origin point is commonly
called the program zero point (also called work zero, part zero, and program
For this example, the two axes we happen to be showing are labeled as X and
Y but keep in mine that program zero can be applied to any axis. Though the
names of each axes will change from one CNC machine type to another (other
common names include Z, A, B, C, U, V, and W), this example should work nicely
to show you how axis motion can be commanded.
The program zero point establishes the point of reference for motion
commands in a CNC program. This allows the programmer to specify movements from
a common location. If program zero is chosen wisely, usually coordinates needed
for the program can be taken directly from the print.
With this technique, if the programmer wishes the tool to be sent to a
position one inch to the right of the program zero point, X1.0 is commanded. If
the programmer wishes the tool to move to a position one inch above the program
zero point, Y1.0 is commanded. The control will automatically determine how
many times to rotate each axis drive motor and ball screw to make the axis
reach the commanded destination point. This lets the programmer command axis
motion in a very logical manner.
With the examples given so far, all points happened to be up and to the
right of the program zero point. This area up and to the right of the program
zero point is called a quadrant (in this case, quadrant number one). It is not
uncommon on CNC machines that end points needed within the program fall in
other quadrants. When this happens, at least one of the coordinates must be
specified as minus.
Understanding absolute versus incremental motion
All discussions to this point assume that the absolute mode of programming
is used. The most common CNC word used to designate the absolute mode is G90.
In the absolute mode, the end points for all motions will be specified from the
program zero point. For beginners, this is usually the best and easiest method
of specifying end points for motion commands. However, there is another way of
specifying end points for axis motion.
In the incremental mode (commonly specified by G91), end points for motions
are specified from the tool's current position, not from program zero. With
this method of commanding motion, the programmer must always be asking
"How far should I move the tool?" While there are times when the
incremental mode can be very helpful, generally speaking, this is the more
cumbersome and difficult method of specifying motion and beginners should
concentrate on using the absolute mode.
Be careful when making motion commands. Beginners have the tendency to think
incrementally. If working in the absolute mode (as beginners should), the
programmer should always be asking "To what position should the tool be
moved?" This position is relative to program zero, NOT from the tools
Aside from making it very easy to determine the current position for any
command, another benefit of working in the absolute mode has to do with
mistakes made during motion commands. In the absolute mode, if a motion mistake
is made in one command of the program, only one movement will be incorrect. On
the other hand, if a mistake is made during incremental movements, all motions
from the point of the mistake will also be incorrect.
Assigning program zero
Keep in mind that the CNC control must be told the location of the program
zero point by one means or another. How this is done varies dramatically from
one CNC machine and control to another. One (older) method is to assign program
zero in the program. With this method, the programmer tells the control how far
it is from the program zero point to the starting position of the machine. This
is commonly done with a G92 (or G50) command at least at the beginning of the
program and possibly at the beginning of each tool.
Another, newer and better way to assign program zero is through some form of
offset. Commonly machining center control manufacturers call offsets used to
assign program zero fixture offsets. Turning center manufacturers commonly call
offsets used to assign program zero for each tool geometry offsets. More on how
program zero can be assigned will be presented during key concept number four.
Other points about axis motion
To this point, our primary concern has been to show you how to determine
the end point of each motion command. As you have seen, doing this requires an
understanding of the rectangular coordinate system. However, there are other
concerns about how a motion will take place. Fore example, the type of motion
(rapid, straight line, circular, etc.), and motion rate (feedrate), will also
be of concern to the programmer. We'll discuss these other considerations
during key concept number three.
Telling the machine what to do - the CNC program
Almost all current CNC controls use a word address format for programming.
(The only exceptions to this are certain conversational controls.) By word
address format, we mean that the CNC program is made up of sentence-like
commands. Each command is made up of CNC words. Each CNC word has a letter
address and a numerical value. The letter address (X, Y, Z, etc.) tells the
control the kind of word and the numerical value tells the control the value of
the word. Used like words and sentences in the English language, words in a CNC
command tell the CNC machine what it is we wish to do at the present time.
One very good analogy to what happens in a CNC program is found in any set
of step by step instructions. Say for example, you have some visitors coming in
from out of town to visit your company. You need to write down instructions to
get from the local airport to your company. To do so, you must first be able to
visualize the path from the airport to your company. You will then, in
sequential order, write down one instruction at a time. The person following
your instructions will perform the first step and then go on to the next until
he or she reaches your facility.
In similar manner, a manual CNC programmer must be able to visualize the
machining operations that are to be performed during the execution of the
program. Then, in step by step order, the programmer will give a set of
commands that makes the machine behave accordingly.
Though slightly off the subject at hand, we wish to make a strong point
about visualization. Just as the person developing travel directions MUST be
able to visualize the path taken, so MUST the CNC programmer be able to
visualize the movements the CNC machine will be making BEFORE a program can be
successfully developed. Without this visualization ability, the programmer will
not be able to develop the movements in the program correctly. This is one
reason why machinists make the best CNC users. An experienced machinist should
be able to easily visualize any machining operation taking place.
Just as each concise travel instruction will be made up of one sentence, so
will each instruction given within a CNC program be made up of one command.
Just as the travel instruction sentence is made up of words (in English), so is
the CNC command made up of CNC words (in CNC language).
The person following your set of travel instructions will execute them
explicitly. If you make a mistake with your set of instructions, the person
will get lost on the way to your company. In similar fashion, the CNC machine
will execute a CNC program explicitly. If there is a mistake in the program,
the CNC machine will not behave correctly.
O0001 (Program number)
N005 G54 G90 S400 M03 (Select coordinate system, absolute mode, and turn
spindle on CW at 400 RPM)
N010 G00 X1. Y1. (Rapid to XY location of first hole)
N015 G43 H01 Z.1 M08 (Instate tool length compensation, rapid in Z to
clearance position above surface to drill, turn on coolant)
N020 G01 Z-1.25 F3.5 (Feed into first hole at 3.5 inches per minute)
N025 G00 Z.1 (Rapid back out of hole) N030 X2. (Rapid to second hole)
N035 G01 Z-1.25 (Feed into second hole)
N040 G00 Z.1 M09 (Rapid out of second hole, turn off coolant)
N045 G91 G28 Z0 (Return to reference position in Z)
N050 M30 (End of program command)
While the words and commands in this program probably do not make much sense
to you (yet), remember that we are stressing the sequential order by which the
CNC program will be executed. The control will first read, interpret and
execute the very first command in the program. Only then will it go on to the
next command. Read, interpret, execute. Then on to the next command. The
control will continue to execute the program in sequential order for the
balance of the program. Again, notice the similarity to giving any set of step
by step instructions.
Other notes about program makeup
As stated programs are made up of commands and commands are made up of word.
Each word has a letter address and a numerical value. The letter address tells
the control the word type. CNC control manufacturers do vary with regard to how
they determine word names (letter addresses) and their meanings. The beginning
CNC programmer must reference the control manufacturer's programming manual to
determine the word names and meanings. Here is a brief list of some of the word
types and their common letter address specifications.
O - Program number (Used for program identification)
N - Sequence number (Used for line identification)
G - Preparatory function
X - X axis designation
Y - Y axis designation
Z - Z axis designation
R - Radius designation
F - Feedrate designation
S - Spindle speed designation
H - Tool length offset designation
D - Tool radius offset designation
T - Tool Designation
M - Miscellaneous function (See below)
As you can see, many of the letter addresses are chosen in a rather logical
manner (T for tool, S for spindle, F for feedrate, etc.). A few require
There are two letter addresses (G and M) which allow special functions to be
designated. The preparatory function (G) specifies is commonly used to set
modes. We already introduced absolute mode, specified by G90 and incremental
mode, specified by G91. These are but two of the preparatory functions used.
You must reference your control manufacturer's manual to find the list of
preparatory functions for your particular machine.
Like preparatory functions, miscellaneous functions (M words) allow a
variety of special functions. Miscellaneous functions are typically used as
programmable switches (like spindle on/off, coolant on/off, and so on). They
are also used to allow programming of many other programmable functions of the
CNC machine tool.
To a beginner, all of this may seem like CNC programming requires a great
deal of memorization. But rest assured that there are only about 30-40
different words used with CNC programming. If you can think of learning CNC
manual programming as like learning a foreign language that has only 40 words,
it shouldn't seem too difficult.
Decimal point programming
Certain letter addresses (CNC words) allow the specification of real numbers
(numbers that require portions of a whole number). Examples include X axis
designator (X), Y axis designator (Y), and radius designator (R). Almost all
current model CNC controls allow a decimal point to be used within the
specification of each letter address requiring real numbers. For example,
X3.0625 can be used to specify a position along the X axis.
On the other hand, some letter addresses are used to specify integer
numbers. Examples include the spindle speed designator (S), the tool station
designator (T), sequence numbers (N), preparatory functions (G), and
miscellaneous functions (M). For these word types, most controls do NOT allow a
decimal point to be used. The beginning programmer must reference the CNC
control manufacturer's programming manual to find out which words allow the use
of a decimal point.
Other programmable functions
All but the very simplest CNC machines have programmable functions other
than just axis motion. With today's full blown CNC equipment, almost everything
about the machine is programmable. CNC machining centers, for example, allow
the spindle speed and direction, coolant, tool changing, and many other
functions of the machine to be programmed. In similar fashion, CNC turning
centers allow spindle speed and direction, coolant, turret index, and tailstock
to be programmed. And all forms of CNC equipment will have their own set of
programmable functions. Additionally, certain accessories like probing systems,
tool length measuring systems, pallet changers, and adaptive control systems
may also be available that require programming considerations.
The list of programmable functions will vary dramatically from one machine
to the next, and the user must learn these programmable functions for each CNC
machine to be used. In key concept number two, we will take a closer look at
what is typically programmable on different forms of CNC machine tools.