Machinery's Handbook, 31st Edition
1360 CNC PROGRAMMING CODES Cutting Speed: The purpose of cutting speed, ( CS ), also known as peripheral speed or surface speed, is to increase or decrease the spindle speed with each change in cutting diameter. The speed will be slowed down for increasing diameters, and speeded up for decreasing diameters. These changes are automatically adjusted by the control system in very fine increments. In order to limit the spindle speed from increasing to potentially dangerous levels at very small diameters, the programmer can limit the maximum spindle speed by using the G50 command. Example: G50 S2500 limit r/min to 2500 in cutting speed mode Example: (G96) G96 S300 M03 cutting speed of 300 ft/min or 300 m/min. G50 is only applicable in G96 mode and has no effect in G97 mode. Its setting should always be less than the maximum spindle speed of the machine. Cutting speed, “CS”, can be converted to spindle speed using the following formulas: US customary units: r/min = (ft/min 3 12) / (3.14 3 diameter in inches) Metric units: r/min = (m/min × 1000) / (3.14 × diameter in mm) The mathematical constant of 3.14 represents mathematical function pi ( π ), rounded to two decimal places, is more than suitable for such calculations. An even shorter formula can be used for US customary units, also suitable for most applications, particularly with out a calculator: r/min = (ft/min 3 4) / Diameter in inches Spindle Override: Spindle override is a feature of CNC machines that allows temporary adjustments to the programmed spindle speed during program execution, without changing the program itself. For this purpose, a spindle override switch is provided at the operation panel. Usually a rotary switch, it is graduated in 10 percent increments, typically between 50 and 120 percent. Permanent changes to the speed must be made in the program itself. Feed Rate Function (F-Address).— Cutting motions are defined as motions of a cut - ter that is in contact with the material, including clearances. Non-cutting motions are typically rapid motions without a physical contact with the material. Programming the feed rate address depends on the type of machine and the units of measurement. Milling machines and machining centers generally use feed rate per minute (inch/min or mm/ min), while lathes and turning centers use feed rate per revolution (inch/rev or mm/rev). For lathes, preparatory commands G94 and G95 determine whether feed rate per minute is selected (G94) or feed rate per revolution is selected (G95). G94 mode—feed rate per revolution—is the default for lathe work. Feed rate specification is always modal, and remains in effect until a different feed rate is selected. Feed rate per revolution (feed/rev) can be converted to feed rate per minute (feed/min) by multiplying spindle speed in revolutions per minute (r/min) by the feed rate per revolution: Feed/min = r/min 3 feed/rev For multi-edge cutters, feed rate is also given as “per tooth” or “per flute.” This feed rate per edge is also generally called “chipload,” specified in inches or millimeters. Feed per tooth (fpt) can be converted to cutting feed rate: Feed/rev = feed per tooth 3 number of teeth Once the feed/rev is known, feed rate per minute can be calculated, if desired. Inverse Time Feed Rate.— One type of feed rate that may be required in some special ap- plications is the inverse time feed rate. This feed rate represents the reciprocal of the time in minutes required to complete a programmed motion. The feed command is indicated by a G93 command followed by an F-address value found by dividing the feed rate, in inches (millimeters) or degrees per minute, by the distance moved in the block: Inverse time feed command = feed rate / distance = (distance / time) / distance = 1 / time The inverse time feed rate has been used in some rotary and multi-axis applications.
Copyright 2020, Industrial Press, Inc.
ebooks.industrialpress.com
Made with FlippingBook - Share PDF online