Copyright Goodheart-Willcox Co., Inc. Chapter 9 CNC Mill Programming 189 The actual starting position can be anywhere off the part, and it might be dictated by the fixture or holding device. Notice that the endpoint of this program is also off the part to prevent any damage to the finished part. 9.5.2 Cutter Compensation A contour toolpath program directs the center of the spindle, or tool, through the Cartesian coordinate points of the part. The diagram in Figure 9-9 represents the path programmed using a 1/2″ end mill from the example code in the previous section. The blue line shows the specified finished dimensions of the part, and the orange shading indicates the tool as it follows that line. This is not what was intended. The finished part, cut to the size of the white section within the orange toolpath, has been cut smaller than the print requirement. The source of this error is the lack of compensation for the diameter of the tool, or cutter compensation. Refer back to the G code list, Figure 9-5. Note the G codes that refer to cutter compensation: ■ G40 turns tool cutter compensation off. ■ G41 moves tool cutter compensation left. ■ G42 moves tool cutter compensation right. From the Shop G41: Left-Hand Compensation Remember from earlier sections, we always want to climb cut with an end mill to stop the tool from grabbing the material, making a rough surface fi nish, or pulling the part out of the fi xture. That means our tool is most often cutting on the left-hand side of the material, or in a G41 cutter compensation. There are a few rare exceptions, but the majority of milling operations use the G41 left-hand compensation. Goodheart-Willcox Publisher Figure 9-9. An illustration of a contour toolpath. The resulting toolpath violates the finished part boundary. Toolpath Tool overcut Intended finished part