Conversational programming considered: advances continue to increase machining efficiencies. (Software Solutions & NC Controls).

The following article is excerpted from the new second edition of Programming of CNC Machines (Industrial Press, New York), by Ken Evans, John Polywka and Stanley Gabrel. The web site for the publisher is http://www .mdustrilpress.com-The Editors

For many years, the concept of programming the CNC machine tool at the controller was thought of as an inefficient and tedious. When orders of a small lot size were to be produced, the choice was almost always manual machines. Today, this is not the case, largely because of the advances in conversational programming.

Conversational programming is becoming more widely used throughout the industry and is available as standard on many machine tool controllers. Its major advantage is that is gives the machinist the ability to write programs at the machine quickly and easily. Typically, the process includes a sequence of questions the machinist/programmer must answer, sometimes called "question answer format" or "prompting." As these questions are answered, the program is constructed. Most controls with this capability also allow the machinist/programmer to graphically check the tool-path to verify the program. If the program has flaws, the controller will not execute the toolpath and the programmer must remedy the problem. When program errors do occur, an alarm number will show on the screen indicating what the problem is and where, in the program, it occurred. This is obviously a better method of finding errors than actually running a part. Another capability of conversational programming is its feature to perform calculatio ns when programming data are missing from the engineering drawing. The programmer constructs intersection points or tangency points and with this information the controller computes the desired geometry. Feeds and speeds are automatically calculated based on the workpiece material and cutting tool material. The data necessary to do this are stored in the controller memory in the cutting condition parameters.

On the floor

Conversational "shopfloor" programming uses the concept of operator prompting combined with a Graphical User Interface (GUI). Questions throughout the programming process prompt the user for information necessary to complete the part program. Icons accessed through the function buttons on the controller identify machining operations, i.e. Point Machining, Line Machining, etc.

Much like CAD/CAM, the process resembles re-creation 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 controlleris 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 G-code 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 conversational programming 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 Maza trol is MNP, where MN stand for Manual and P for Programming.

There are many different conversational languages for programming available, and one of the complaints is the lack of standardization between the various machine tool builders. The industry leader in conversational programming has always been Mazak with its 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.

Program creation

What follows are brief descriptions of the programming process for turning centers.

The control must be in the program-editing mode and a work number (program number) must be identified. 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 type of program to create either Mazatrol or EIA/ISO must be determined. All Mazak machines use Mazatrol as their standard with EIA/ISO (G-Code) as an optional feature. The turning center programs are made up of these four basic parts: Common Data Process, Machining Process, Sequence Data and End Process.

The information at the head of the program applies to the entire program. The programmer is prompted to answer the following questions for this common data.

What is the material?

The controller is preset with standard materials of carbon steel, alloy steel, cast iron, aluminum and stainless to choose from. This choice affects the automatic calculation of cutting feeds and speeds throughout the program.

What is the maximum outer diameter of the workpiece?

This value is dependent upon the diameter geometry of the raw workpiece. If the programmer inadvertently exceeds this diameter with any values in the program, the controller will set off an alarm preventing execution of toolpath verification and automatic operation.

What is the minimum inner diameter of the workpiece?

If the workpiece geometry is of solid bar stock, this value may be set to zero. If an inner diameter exists, the programmer must input this value. Doing this prevents the generation of toolpath where material is nonexistent.

What is the overall length of the workpiece?

The overall length of the workpiece along the Z axis, including the clamping amount should be entered for this value. If a programmed value exceeds this length, the controller will set off an alarm preventing execution of toolpath verification and automatic operation.

Would you like to limit the spindle RPM to a maximum?

If no value is input into this data slot, the controller will execute the maximum spindle RPM when at the centerline in the X axis. This maximum RPM may be undesirable in some cases.

Would you like to limit the spindle RPM to a maximum?

This enables the programmer to limit the spindle RPM to a predetermined amount. If no value is input into this data slot, the controller will execute the maximum spindle RPM when at the centerline in the X axis. This maximum RPM may be undesirable in some cases.

How much material would you like to leave for a finish pass in the X axis?

The amount of material to be left for a finishing pass in the X axis is input at this time. This value is input in consideration of the diameter of the work-piece. For example: if a value of 0.040 is input, the amount taken off the diameter is equal to 0.080 for the finishing pass.

How much material would you like to leave for a finish pass in the Z axis?

The amount of material to be left for a finishing pass in the Z axis is input at this time.

What is the amount of material taken off the work face to attain Z zero?

It is common to machine from the face of the workpiece in order to attain a finished surface that establishes the Z zero for the part. This amount is dependent upon the condition of the material and programmer preference.

Machining process

At this point, the individual machining process data are identified in order to complete the workpiece definition. In other words, what type of machining is to be done? The choices are BAR, CPY, CNR, EDG, THR, GRV, WORKPIECE SHAPE and END.

Bar (BAR) machining is used for outside diameter (OD) or, inside diameter (ID) turning and boring. Copy (CPY) machining is used for OD or ID machining of existing geometries like castings or forgings, where a uniform amount of material is to be removed and is other than solid bar stock. Corner (CNR) machining is used when additional cutting tools are needed to finish corners that cannot be cut because of tool geometry limitations. Edge (EDG) machining is used to perform machining on the face of the workpiece. Thread (THR) is for machining of external and internal grooves. Workpiece shape machining is similar to CPY except that the material removal shape does not need to be uniform. END is used to end the program.

Sequence data

The finished workpiece shape is identified by input of point data until the desired geometry exists using lines (LIN), tapers (TPR), arcs, chamfers and fillets, limited only by the tool configuration. The same type data are necessary for internal bar machining. In the figure below, the two types of arcs shown represent convex and concave shapes respectively and the CENTER command is needed to identify the arc center point.

When all the geometric data are entered and the shape is defined properly, then the SHAPE END function key is pressed to end the process. The remainder of the program is constructed in the same manner until complete.

At End

End-this process ends the program (similar to M30 in G-Code programming) and offers the opportunity to the programmer to: set a counter for the number of workpieces to be machined, set the return position of the turret after machining ends; identify a next program number to machine, whether to continue the same program repeatedly or not, and how many repetitions; also, the shift amount for the coordinates system can be set.

Other steps

Once the program data are entered, the programmer may perform a shape check of the geometry to verify its accuracy. The controller will not allow the shape check if there are serious problems with the geometry and an alarm will be displayed on the screen identifying the program number, process number and sequence number of the mistake. Performing a shape check will draw the finished workpiece geometry on the screen in two-dimensional form.

Another step is toolpath verification. The newest controllers are equipped with solid model rendering of the workpiece raw stock configuration. The programmer can simulate onscreen, the actual machining of the workpiece in real time by pressing check continue.

Once the verification steps are complete, the machinist may begin the first article of CNC automatic operation.

For machining centers

Following are brief descriptions of the programming process for machining centers. The control must be in the program-editing mode and a work number (program number) must be identified. 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 type of program to create either Mazatrol or EIA/ISO must be determined. All Mazak machines use Mazatrol as their standard with EIA/ISO (G-Code) as an optional feature. The construction of a Mazatrol machining center program contains these basic parts: a common data unit, identification of a coordinate system, the machining units and their sequence data and an End unit.

The future

The ultimate goal of any manufacturing is to increase productivity by improving efficiency. Minimizing wasted and idle time to cut lead times while maintaining accuracy. Modem technology enables these goals to become reality.

The PC has revolutionized our society, and manufacturing has been a benefactor because of the direct effect on controlling CNC machines. Now PCs are used to network machines together, in order to manage workloads. These networks also make it possible to communicate between machines and the office to manage and download programs, to obtain machine status and operation reports in real time, and monitor other network locations. Machine monitoring includes automatic operation, machine stop and feed hold, set-up and alarm. Spindle load and spindle speed are recorded to provide reports and information on completed workpiece counts. Some machines utilize both a PC and CNC fused into one, providing bi-directional communication between PC and CNC. This makes an intelligent CNC control system. Intelligent CNC responds to questions, makes suggestions and provides detailed reports on machine operation and production status.

The most advanced RISC CPU (Reduced Instruction Set Computer, Central Processing Unit) technology is used providing faster processing speeds which, in turn, help to achieve reduced set-up and cycle times.

Knowledge-based navigation functions allow the determination of optimum metal cutting conditions prior to actual cutting, dependant upon stored data. Based on the part program, tool data and workpiece material, the navigation functions suggest the optimum cutting conditions and shows where improvements in cycle time can be achieved through changes in spindle speed, feedrate and tools.

Advancements in the graphical cutting simulation allow the 3D solid part model to be displayed. This feature can be used to show part sections for checking inside diameters and deep holes, and views can be rotated. These added capabilities aid in program verification of toolpaths.

To keep machine utilization high, modem controls allow self-diagnostic functions for service and maintenance. Self-diagnostic menus quickly trouble shoot the cause of an alarm and suggest possible solutions for trouble-shooting. Alarm displays indicate when scheduled maintenance is required and on-line support is available.

As technological advancements continue at an unbelievable pace the manufacturing industry will undoubtedly benefit. Innovative new methods for CAD/CAM and conversational programming of CNC machines will continue to emerge. For the machinist/programmer this means that the new methods and tools used for programming will require a life-long learning approach.