C OMMON D ATA P ROCESS

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

WORKPIECE MATERIAL <Menu>

The controller memory is preset with standard materials of Carbon Steel, Alloy Steel, Cast Iron, Aluminum and Stainless Steel to select from in the menu. This choice affects the automatic calculation of cutting feeds and speeds throughout the program. It is possible to add user defined materials to the cutting condition parameters if the material needed is not available.

MAX. OUTER DIA. of WORKPIECE

This value input here is dependant upon the diameter geometry of the raw workpiece. Note: If the programmer inputs a value that exceeds this diameter, an alarm will result on the controller display which will prevent execution of tool path verification and automatic operation.

MIN. INNER DIA. of WORKPIECE

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

WORKPIECE LENGTH

The overall length of the workpiece along the Z axis, including the clamping amount, should be entered for this value. It must be at least the maximum machined length. If a programmed value exceeds this length, the controller will set off an alarm display preventing execution of tool path verification and automatic operation. This value is not meant to represent the extension value for the setup of the part in the chuck jaws.

MAX. SPINDLE RPM LIMIT (rpm)

This enables the programmer to limit the spindle RPM to a predetermined amount (G50 in G-Code programming). If no value is input into this data field, 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.

FINISH ALLOWANCE-X

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 workpiece. For example: if a value of .040 inch is input, the amount taken off the diameter is = to .080 inch for the finishing pass.

FINISH ALLOWANCE-Z

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

STOCK REMOVAL of WORKFACE

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

M ACHINING P ROCESS

In this section, of the program, the individual machining process data are identified in order to complete the workpiece definition. In other words, what the type of machining that is is to be done. In the Figure 3 below, note the choices are BAR, CPY, CNR, EDG, THR, GRV, WORKPIECE SHAPE and END.

Figure 3 Machining Process Menu

Bar ( BAR ) machining is used for outside diameter (O.D.) or, inside diameter (I.D.) turning and boring. Copy ( CPY ) machining is used for O.D. or I.D. 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 screw threads. Grooving ( GRV ) 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. The arrow keys at the right offer some additional options of Drilling, Tapping and Manual Programming (as mentioned above i.e.

G-Code within the Mazatrol program).

Once a selection is made for the type of machining operation, then more information is needed to identify how to apply it. In Figure 4 below, BAR machining has been selected and a new set of menu choices are displayed. Those items that are bold in the graphic are captured-type of cuts. The first on the left, OUT , is used to perform general O.D. machining and the third from the left, IN , is used for general I.D. machining like boring.

Figure 4 BAR Machining Menu

Once the type of machining is selected ( BAR) , the necessary related information is as follows: Feeds and Speeds, are automatically calculated by pressing a function soft key (AUTOSET) and are based on parameter information directly associated to the selected cutting tool and workpiece material identified in the Common Data Process; tool selection for roughing and finishing cycles; the Starting Point in X ( SPT-X ); the Starting Point in Z ( SPT-Z ); the Finish Point in X ( FPT-X ) and, the Finish Point in Z ( FPT-Z ).

Sequence Data

The finished workpiece shape is identified by the input of point data until the desired geometry exists using lines ( LIN ), tapers ( TPR ), arcs, chamfers and fillets, limited only by the tool geometry configuration. The same type data are necessary for internal bar machining. In Figure 5 below, the two types of arcs shown represent convex and concave shapes, respectively, and the CENTER menu selection command is needed to identify the arc center point.

Figure 5 Sequence Data Menu

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