CNC Info

2011-01-08T03:19:00.001-08:00

The abbreviation CNC stands for computer numerical control, and refers specifi cally to a computer

“controller” that reads G-code instructions and drives a machine tool, a powered mechanical device

typically used to fabricate components by the selective removal of material. CNC does numerically

directed interpolation of a cutting tool in the work envelope of a machine. The operating parameters of

the CNC can be altered via software load program.

CNC was preceded by NC (Numerically Controlled) machines, which were hard wired and their operating

parameters could not be changed. NC was developed in the late 1940s and early 1950s by

John T. Parsons in collaboration with the MIT Servomechanisms Laboratory. The fi rst CNC systems

used NC style hardware, and the computer was used for the tool compensation calculations and

sometimes for editing.

Punched tape continued to be used as a medium for transferring G-codes into the controller for many

decades after 1950, until it was eventually superseded by RS232 cables, fl oppy disks, and now is

commonly tied directly into plant networks. The fi les containing the G-codes to be interpreted by the

controller are usually saved under the .NC extension. Most shops have their own saving format that

matches their ISO certifi cation requirements.

The introduction of CNC machines radically changed the manufacturing industry. Curves are as easy

to cut as straight lines, complex 3-D structures are relatively easy to produce, and the number of machining

steps that required human action has been dramatically reduced.

With the increased automation of manufacturing processes with CNC machining, considerable improvements

in consistency and quality have been achieved with no strain on the operator. CNC automation

reduced the frequency of errors and provided CNC operators with time to perform additional

tasks. CNC automation also allows for more fl exibility in the way parts are held in the manufacturing

process and the time required to change the machine to produce different components.

In a production environment, a series of CNC machines may be combined into one station, commonly

called a “ cell”, to progressively machine a part requiring several operations. CNC machines today are

controlled directly from fi les created by CAM software packages, so that a part or assembly can go

directly from design to manufacturing without the need of producing a drafted paper drawing of the

manufactured component. In a sense, the CNC machines represent a special segment of industrial

robot systems, as they are programmable to perform many kinds of machining operations (within

their designed physical limits, like other robotic systems). CNC machines can run over night and over

weekends without operator intervention. Error detection features have been developed, giving CNC

machines the ability to call the operator’s mobile phone if it detects that a tool has broken. While the

machine is awaiting replacement on the tool, it would run other parts it is already loaded with up to

that tool and wait for the operator. The ever changing intelligence of CNC controllers has dramatically

increased job shop cell production. Some machines might even make 1000 parts on a weekend with

no operator, checking each part with lasers and sensors.

Introduction to CNC

Types of instruction

A line in a G-code fi le can instruct the machine tool to do one of several things.

Movements

The most basic motion for a controller is to move the machine tool along a linear path from one point

to another. Some machine tools can only do this in XY, and have to accept changes in Z separately.

Some have two further axes of rotation to control the orientation of the cutter, and can move them

simultaneously with the XYZ motion. Lately 4 and 5 axis machines have become popular. The 2 additional

axis allow for the work surface or medium to be rotated around X and Y. For example, a 4-axis

machine can move the tool head in XY and Z directions, and also rotate the medium around the X or

Y axis, similar to a lathe. This is called the A or B axis in most cases.

All motions can be built from linear motions if they are short and there are enough of them. But most

controllers can interpolate horizontal circular arcs in XY.

Lately, some controllers have implemented the ability to follow an arbitrary curve ( NURBS), but these

efforts have been met with skepticism since, unlike circular arcs, their defi nitions are not natural and

are too complicated to set up by hand, and CAM software can already generate any motion using

many short linear segments.

With the advent of the vortech router cnc quad drive system which utilizes four (bidirectional) motors

and drive, users are able to achieve greater speeds and accuracy.

Drilling

A tool can be used to drill holes by pecking to let the swarf out. Using an internal thread cutting tool

and the ability to control the exact rotational position of the tool with the depth of cut, it can be used to

cut screw threads.

Drilling cycles

A drilling cycle is used to repeat drilling or tapping operations on a workpiece. The drilling cycle accepts

a list of parameters about the operation, such as depth and feed rate. To begin drilling any number

of holes to the specifi cations confi gured in the cycle, the only input required is a set of coordinates

for hole location. The cycle takes care of depth, feed rate, retraction, and other parameters that appear

in more complex cycles. After the holes are completed, the machine is given another command

to cancel the cycle, and resumes operation.

Parametric programming

A more recent advancement in CNC interpreters is support of logical commands, known as parametric

programming. Parametric programs incorporate both G-code and these logical constructs to create

a programming language and syntax similar to BASIC. Various manufacturers refer to parametric

programming in brand-specifi c ways. For instance, Haas refers to parametric programs as macros.

GE Fanuc refers to it as Custom Macro A & B, while Okuma refers to it as User Task 2. The programmer

can make if/then/else statements, loops, subprogram calls, perform various arithmetic, and

manipulate variables to create a large degree of freedom within one program. An entire product line of

different sizes can be programmed using logic and simple math to create and scale an entire range of

parts, or create a stock part that can be scaled to any size a customer demands.

Parametric programming also enables custom machining cycles, such as fi xture creation and bolt

circles. If a user wishes to create additional fi xture locations on a work holding device, the machine

can be manually guided to the new location and the fi xture subroutine called. The machine will then

drill and form the patterns required to mount additional vises or clamps at that location. Parametric

programs are also used to shorten long programs with incremental or stepped passes. A loop can be

created with variables for step values and other parameters, and in doing so remove a large amount

of repetition in the program body.

Because of these features, a parametric program is more effi cient than using CAD/CAM software for

large part runs. The brevity of the program allows the CNC programmer to rapidly make performance

adjustments to looped commands, and tailor the program to the machine it is running on. Tool wear,

breakage, and other system parameters can be accessed and changed directly in the program, allowing

extensions and modifi cations to the functionality of a machine beyond what a manufacturer envisioned.

There are three types of variables used in CNC systems: Local variable, Common variable, and

System variable. Local variable is used to hold data after machine off preset value. Common variable

is used to hold data if machine switch off does not erase form data. The System variable this variable

used system parameter this cannot use direct to convert the common variable for example Tool

radius, Tool length and tool height to be measured in mm or inches.

Introduction to CNC

There are other codes; the type codes can be thought of like registers in a computer

• X absolute position

• Y absolute position

• Z absolute position

• A position (rotary around X)

• B position (rotary around Y)

• C position (rotary around Z)

• U Relative axis parallel to X

• V Relative axis parallel to Y

• W Relative axis parallel to Z

• M code (otherwise referred to as a “Miscellaneous” function”)

• F feed rate

• S spindle speed

• N line number

• R Arc radius or optional word passed to a subprogram/canned cycle

• P Dwell time or optional word passed to a subprogram/canned cycle

• T Tool selection

• I Arc data X axis

• J Arc data Y axis.

• K Arc data Z axis, or optional word passed to a subprogram/canned cycle

• D Cutter diameter/radius offset

• H Tool length offset

2 Axis Fundamentals

Fundamentals of G-Code

G-Code programming is a very simple programming language. When we were kids, we used to and

may still do connect the dot puzzle games. G-code works exactly on the same principle. It takes two

simple concepts to understand G-code programming, connect-the-dots and the number line.

Connect-the-dots

We can draw something very simply by connecting the dots.

We do not think about it, but we are creating something tangible in the

2-axis world.

The Number Line

The number line is simply the measurement of units. Let’s look at this number line:

-2 -1 0 1 2

In a straight line numbers either get bigger or smaller from Zero. Machining, along with G-Code programming,

uses both sides of Zero.

Signs +/ -

The Plus (+) sign and the Minus (-) sign are very important in machining. In machining we can also

call them Positive or Negative respectively. We use these signs in two situations; location and direction.

Location

They signify what side of Zero a number is on, we can say this is a location indicator; Left for Minus

and Right for Positive respectively from Zero.

Direction

These signs also are used as a tool to tell us which direction to move; Left for Minus and Right for

Positive.

Introduction to G-Code

Standard G-Codes - Mill

The G-Codes are what tell the machine to do with positional reference. This is just a simple reference

to what standard G-Codes do.

G0 or G00 – Rapid Movement

The fastest the Machine can go to the next defi ned position. If moving in multiple axis, each axis will

move as fast as they can independently of one another until it reaches it’s defi ned end points.

G1 or G01 – Linear Movement

A straight line move with a speed defi ned by an F. If moving in multiple axes, the machine will move

proportionally in each axis until it reaches its defi ned end position.

G2 or G02 – Interpolation Clockwise

A circular movement in 2 axis. Will create an arc to a specifi ed radius defi ned by R or I/J.

G3 or G03 - Interpolation Counter Clockwise

A circular movement in 2 axis. Will create an arc to a specifi ed radius defi ned by R or I/J.

G4 or G04 – Dwell

Machine will dwell once reached position to a user defi ned time, P.

G9 or G09 – Exact Stop/ Exact Position

Machine will not traverse to next line of code until it positions exactly to position.

G10 - Data Setting

G17 - XY plane selection

G18 - ZX plane selection

G19 - YZ plane selection

G20 - Machine in inch

G21 - Machine in MM

G28 - Return to Reference Position

Normally machine home.

G30 - Return to 2nd reference position

Normally pallet changing/tool change home if different than machine home.

G40 - Cutter Compensation Cancel

G41 - Cutter Compensation Left

Used with user defi ned value, D

G42 - Cutter Compensation Right

Used with user defi ned value, D

G43 - Tool Length Compensation +

Used with user defi ned value, H. Common

G44 - Tool Length Compensation -

Used with user defi ned value, H. Not common

G49 - Tool Length Compensation Cancel

Part1 Tutorial

This is a sample part tutorial to begin basic milling programming. Included is a sample print, Part1,

and a G-Code program to make the part.

The following is a detailed explanation of a standard Fanuc programmed part.

This program is a Milling program, programmed to the side of the tool.

The Part Zero for programming purposes of this part are:

X0 = Left Edge of Part

Y0 = Bottom Edge of Part

Z0= Top of Part

* Refer to print on following page.

***All Feeds and Spindle speeds and reference information are from the book

“CNC Programming - Reference Book”

119

Part1 Tutorial

G-Code Program

O0001(PROGRAM#)

(PROGRAM NAME - PART1)

(SAMPLE PART)

N1( 1” FLAT ENDMILL TOOL )

T1M6

N100G0G90G54X-1.Y0.S3056M3

G43H1Z.1M8T2

(PROFILE)

G1Z-1.F24.4

G41D51X-.5

Y1.75

G2X.25Y2.5I.75

G1X3.5

G2X4.5Y1.5J-1.

G1Y.75

G2X3.25Y-.5I-1.25

G1X0.

G2X-.5Y0.J.5

G1G40X-1.

G0Z.1

(FINISH WALL STEP3)

X1.25Y4.5

G1Z-.5

G41D51Y4.

G2X3.5Y1.75J-2.25

G1Y.25

G2X1.25Y-2.I-2.25

G1G40Y-2.5

G0Z.1

(FINISH WALL STEP 2)

Y3.75

G1Z-.5

G41D51Y3.25

G2X2.75Y1.75J-1.5

G1Y.25

G2X1.25Y-1.25I-1.5

G1G40Y-1.75

G0Z.1

(FINISH WALL)

Y3.

G1Z-.5

G41D51Y2.5

G2X2.Y1.75J-.75

G1Y.25

G2X1.25Y-.5I-.75

G1G40Y-1.

G0Z.1M9

G91G28Z0M19

N2(5/8 SPOT DRILL TOOL )

(1/2-13)

T2M6

N200G0G90G54X.75Y1.S2500M3

G43H2Z.1M8T3

G98G81Z-.25R.1F10.

(.375 DIAMETER)

X2.5Z-.6875R-.4

G80Z.1M9

G91G28Z0M19

N3( 27/64 DRILL TOOL)

(1/2-13 DRILL)

T3M6

N300G0G90G54X.75Y1.S2264M3

G43H3Z.1M8T4

G98G83Z-1.2267R.1Q.2109F9.

G80Z.1M9

G91G28Z0M19

N4(1/2-13 CUT TAPRH TOOL )

T4M6

N400G0G90G54X.75Y1.S130M3

G43H4Z.1M8T5

G84Z-1.35R.1F10.

G80Z.1M9

G91G28Z0M19

N5( #U DRILL TOOL, .368)

(.375 DRILL)

T5M6

N500G0G90G54X2.5Y1.S2595M3

G43H5Z.1M8T6

G98G83Z-1.2106R-

.4Q.184F10.4

G80Z.1M9

G91G28Z0M19

N6(.375 REAMER TOOL, .375)

(.375 REAM)

T6M6

N600G0G90G54X2.5Y1.S1000M3

G43H6Z.1M8T1

G98G85Z-1.2R-.4F10.

G80Z.1M9

G91G28Z0M19

G28Y0

M30

CNC INFO

CNC Info