CNC

14 Sep

Example of NC part programming (2D contouring)

This is part two of Workshop Technology Manual CNC Machining

Figure 3: Sample Part

We assume that the machining is a contouring operation along the outer boundary of a simple part, whose nominal geometry is as shown on Fig.3.

The tool size is 0.25 inch, and the feed rate of 6 inch per minute is used.

The cutting speed is required to be 300 rpm. To simplify the program, we ignore the Zaxis motions, and that the home position of the tool is at the correct height, centered on the point located in the machine tool coordinates as (2, 2).

In order to specify the geometry of the motion, we need to compute the location of 5 points from p1 to p5 (later, we shall see that additional points will be needed).

The cutting will proceed along the contour: p0 -> p1 -> p2 -> p3 -> p4 -> p5 -> p1.

// Block 1: start program, use absolute coordinates, spindle speed in rpm, feed in inch/min, select tool no 1001, turn coolant ON, use up milling (CCW in this case)

N010 G70 G90 G94 G97 M04[EOB]

NOTE: we could use M14 instead of M04 and M08 that we shall use in the next block.

// Block 2: cutting on XY plane, set feed, spindle speed,

N020 G17 F6.0 S300 T1001 M08 [EOB]

// Block 3: move to first point in a straight line (linear interpolation). We now need to compute the coordinates of p1, as shown in figure below:

Figure 4 : Calculating p1 coordinate

N030 G01 X3.875 Y3.698 [EOB]

// Block 4: move to p2 in straight line. coordinates of point p2: x = same as p1; y = 4 + 5 + 0.125.

N040 G01 X3.875 Y9.125 [EOB]

// Block 5: move to p3. coordinates calculated as shown in figure below:

Figure 5 : Calculating p3 coordinate

N050 G01 X5.635 Y9.125 [EOB]

// blocks 6, 7, 8: now we need to cut along a circular arc.

Most NC controllers cannot cut along a full circle directly — they need to be programmed once FOR EACH QUADRANT of the arc. In our case, the circular path of the tool goes through tree quadrants, so we need to find two additional points, p31, and p32.

Programming for circular interpolation (moving the tool along a circular arc): Circular arcs are machined only in main planes. The plane is selected by the preparatory functions (G17, G18, G19). The direction of the tool along the arc must be specified (G02, G03, G20 G21, G30, G31).

Four dimension words are needed per block. Two dimension words specify the distance to the end of the arc from current position. Two circular dimension words specify the distance to the arc center. Usually, I, J, K specify the distances parallel to the X, Y, Z axes, respectively.

The I, J, K values are absolute values (unless there is ambiguity). The following figure shows the computations of the next three blocks of motion: