Machinery's Handbook, 31st Edition
CNC PROGRAMMING CODES 1361 Feed Rate Override.— The feed rate override is a feature of CNC machines that allows temporary adjustments to the programmed cutting feed rate during program execution, without changing the program itself. For this purpose, a feed rate override switch is pro vided at the operation panel. Usually a rotary switch, it is graduated in 10 percent incre- ments, typically with a range of 0 to 150 or 200 percent. Permanent changes to the feed rate must be made in the program itself. Tool Function (T-Address).— Both CNC milling and turning machine groups use automatic tool change (ATC). In the program, each tool has to be numbered using the T-address. On machining centers, tools are stored in a special tool magazine, located on a side of the machine. On lathes, tools are stored in an indexing turret, located within the machining area. There is a difference in programming each group. In both groups, the T-address indicates the tool number of the next tool. For example, on a machining center, T06 is tool number six. Tools can be stored in any magazine position, but must be regis- tered in the control system prior to use. On lathes, the four-digit tool number is determined by the turret station number, followed by a wear offset number. The turret station number is also equivalent to the geometry offset for the stored tool. Wear offset is used for fine- tuning. For example T0313 calls a tool located in turret station three, activates geometry offset three as well as work offset thirteen. Tool offset screens (geometry and wear) are special tables visible on the control display panel that show the setting information about each tool. Such information includes the XZ setting, tool nose radius (R), and the tool tip number (T) which should not to be confused with tool number. Tool Nose Radius Compensation.— A typical manually generated program uses both coor- dinate points read directly from drawings and calculated on the basis of drawing dimensions. In both cases, these calculated coordinate points represent a toolpath along the part edge suit- able only for a cutter that has a radius of zero. Since a zero tool radius is not practical, the tool’s actual radius has to be considered. This is achieved by using a powerful control feature called cutter radius offset (compensation) or—for lathe terms—tool nose radius compensation. During program development, the programmer ignores the cutter radius, and uses drawing based dimensions. In order to allow for radius compensation at the machine, two preparatory commands are used—G41 for the compensation to left, and G42 for the compensation to the right. In both cases, the direction is determined by viewing along the cutter path direction. At the control, the operator sets not only the XZ geometry and wear offsets, but also enters the tool nose radius (R-column) and the tool tip number (T-column). The purpose of the tool tip number is to establish the location of the tool nose radius center point.
Radius
T2
T1
T6
Setup point
T7
T0
T5
Radius
T8
T3
T4
Setup point
Fig. 4. Tool Tip Numbers—Rear Lathe. Rapid Motion (G00).— In basic terms, machine motions are divided into two groups, non- cutting motions (unproductive) and cutting motions (productive). Rapid motion is the only
Copyright 2020, Industrial Press, Inc.
ebooks.industrialpress.com
Made with FlippingBook - Share PDF online