Copyright Goodheart-Willcox Co., Inc. Chapter 9 CNC Mill Programming 191 into X0., while turning on the G41. Second, designate the offset used (D1 in the given example) and enter the tool diameter in the tool offset page, Figure 9-11. This entry is your diameter offset. Some machines may be set to radius instead of diameter. See the user manual to change this setting, or use the radius of the tool as the offset. Diameter Offsetting The diameter offset in your control can be a very useful function. The pre- vious example shows how easy it becomes to program a path if there are no calculations needed for the tool diameter. In a machine shop environ- ment, it is sometimes necessary to use a tool with a different diameter than originally specified in the program. If a program is written for a 1/2″ end mill, but the only end mills available are 5/8″, you would have to start a new program to accommodate the difference in size. With the control cal- culating G41 or G42 positions, it is a simple matter to go back to the tool offset page and change the diameter geometry offset to .625″. Another benefit to using diameter offsetting is the ability to make small, incremental changes. In our example print and program, this part is defined as a 6.000″ × 3.000″ rectangular part. But what if this piece comes out to 6.010″ × 3.010″? The machinist can make a small change to the .500″ tool diameter offset to make the part either bigger or smaller. Define the tool as .490″ diameter (or smaller) to move the path closer into the part and cut the part smaller. Remember, the machine is cutting lines on both sides of the rectangle, so moving in the tool will affect both sides. This function can also serve as a setup technique in creating the first part to help prevent cutting that part undersize. Change the tool to .550″ diameter offset so that the machine calculates the path farther away from the programmed dimensions, thus leaving the part larger. After the pro- gram is complete, measure the part and offset the tool to reach the desired final size. After the diameter offset is altered and the correct size is achieved, all subsequent parts can be machined at the new diameter offset value. 9.6 Radius and Angle Milling While contours are the most common toolpath, even in simple contoured parts there are often radii and angles to be programmed. The advent of better control technology has simplified this once complex programming task. This section will discuss the G02 and G03 codes used to create arcs as well as the I, J, and K method (used in older controls or to create circles). Goodheart-Willcox Publisher Figure 9-11. The tool offset screen where the tool diameter is entered. PROBING TOOL 1 OFFSET 1 SPINDLE 2 3 4 5 6 7 8 9 10 0 0 0 0 0 0 0 0 4.5680 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. 0. POSITION GEOMETRY WEAR GEOMETRY WEAR COOLANT H(LENGTH) D(DIA) TOOL OFFSET TOOL INFO