Much like CAD/CAM, the programming process resembles recreation of the part geometry by constructing the shapes using lines, arcs, and points combined with other features.

This information is used in combination with Tool Identification Parameters and Cutting Condition Parameters to generate the tool path code needed to control the machine. The programmer has the added functions of the controller’s ability to calculate for unknown coordinate values and have them automatically inserted into the program where they are needed. In most cases, no calculator is needed for trigonometric calculations. These constructions resemble the formerly popular Automatic Programmed Tool ( APT ) method of programming. The actual program the machine executes is still a GCode format but the operator may never see the actual code on the display.

This type of programming combined with the ability to call G-Code sub programs has tremendous power. Mazatrol, a conversationalprogramming system offered on all MAZAK machine tools allows “G-Code similar” programming, within its conversational language, in what is called a Manual Programming Process. The acronym used to call this type of program process for Mazatrol is MNP , where MN stands for Manual and P for Programming.

There are many different conversational languages available for programming available, and one of the main complaints has been is the lack of standardization between the various machine tool builders. MAZAK’s Mazatrol language has been at the forefront of the industry in conversationalprogramming for decades and has a proven track record of success has always been MAZAK with their Mazatrol language. The focus of this chapter will be centered on this language only. Other languages contain similar techniques that accomplish nearly the same result.

Just as with any programming endeavor, you must be well prepared. The sequence of events followed by the programmer programmer in order to create a Mazatrol program are very similar to those used in manual programming. Careful examination Study of the technical part drawing for, work holding considerations and tool selection must take place prior to preparation of the part program. With that in mind, it is most efficient to establish a Tool File within the Mazak controller prior to programming. This file should contain a representation of the tools that are available to choose from in your shop. From this information, one of the more powerful aspects of Mazatrolconversationalprogramming can be used to automatically develop tools used in the program. This tool definition, when properly defined, can also be used to automatically calculate

the proper feeds and speeds used for machining. Once this file is setup, programming may begin.

When the program is completed, the tool path must be verified by graphical simulation. At this point, if all checks well, the operator takes over for the measuring of tool and work offsets and one final program test by dry run. And, finally, the first part of CNCmachining begins.

C ONVENTIONS

For this section, the following text format convention is used. For the MENU selection, the letters will be in CAPITALS while the user prompts will be in capital ITALICS. Mazatrol acronyms are given in capital letters and BOLD TYPE.

TURNING CENTER PROGRAM CREATION

During the programming process, many unique abbreviations and acronyms are used to simplify prompting and input. The following are some of the acronyms encountered in the sequence of creating MazatrolconversationalTurning Center programs:

T URNING C ENTER A BBREVIATIONS AND A CRONYMS

WKNO = Workpiece Number

MAT = Material

FC = FerrousCast Iron

FCD = Ferrous Cast Ductile Iron

S45C = Low Carbon Steel

SCM = Alloy Steel

SUS = Stainless Steel

AL = Aluminum

CU = Copper

CB ST = Carbon Steel

ALOY = Alloy Steel

CASIR = Cast Iron

9310 = 9310 Alloy Steel

BRASS = Brass

A2 = Tool Steel

MAX = Maximum

MIN = Minimum

OD = Outside Diameter

ID = Inside Diameter

RPM = Revolutions per Minute

FIN-X = Finish Allowance - X axis

FIN-Z = Finish Allowance - Z axis

BAR = Bar Machining e.g. solid Barstock

CPY = Copy Machining i.e. net shape material, casting, etc. Uniform material all

around, all surfaces

CNR = Corner Machining e.g. re-machining of corners where the tool cannot reach,

due to tool geometry + more

EDG = Edge Machining

FCE = Face

BAK = Back

THR = Threading Inside Diameter (I.D.) or Outside Diameter (O.D.)

GRV = Grooving, I.D., O.D., Face or Back

MTR = Workpiece Shape, is a user defined arbitrary shape that is other than bar

or net shape and requiring non-uniform material removal

DRL = Drill

MNP = Manual Program Unit

M-CODE = Miscellaneous codes e.g. coolant M8

FCE = Face e.g. Edge FCE or BAR FCE

CPT-X = Cutting Point - X axis

CPT-Z = Cutting Point - Z axis

RV = Surface Speed for Rough Cut (V = Velocity)

FV = Surface Speed for Finish Cut (V = Velocity)

V ROUGHNESS = Surface Roughness determined by in/rev setting

R-FEED = Roughing Feed rate in/rev or mm/rev

R-DEP = Roughing Maximum Depth of Cut

R-TOOL = Rough Tool No.

F-TOOL = Finish Tool No.

ID CODE = Tool Identification Code for Spare Tool Usage

LIN = Linear Feed Move

TPR = Tapered Feed Move

S-CNR = Start <CNR-C> or <CNR-R> This means Start Corner -C = Chamfer -

R = radius

SPT-X = Geometry Starting Point - X axis

SPT-2 = Geometry Starting Point - Z axis

FPT-X = Geometry Final Point - X axis

FPT-2 = Geometry Final Point – Z axis

F-CNR = Final <CNR–C> <CNR-R>/Necking Final corner chamfer or radius or

necking

CTR = Center Point for Radius Programming

BAK = Back Machining

CHAMF = Chamfer for thread ending

ANG = Angle of thread

HGT = Thread Height

V = Velocity Cutting SpeedThreading

END = End Unit

SHIFT = Second/third part, etc., shift amount

TPC = Temporary Parameter Change/Toolpath Control

Following, are brief descriptions of the general programming process for Turning

Centers:

The control must be in the program-editing mode and a work number (program

number) must be identified in order to begin.

• Press the soft key labeled “Work No.” and key in the desired program number,

and press Input.

Note: There is no need for the letter address O to precede the program number with Mazatrol programs.

Before any programming can take place, the programmer must determine the type of program needed EIA/ISO or Mazatrol. All MAZAK machines use Mazatrol as their standard program type, with EIA/ISO (G-Code) on some older generation machines as an optional feature. Turning Center programs are made up of these four basic parts; a Common Data Process, Machining Process, Sequence Data and an End Process.