Machinery's Handbook, 31st Edition
1376 CNC THREAD CUTTING Using the compound threading method, a heavier pass depth with fewer passes can be used for majority of threads. Compound infeed can be modified by providing 1 to 2 degrees of clearance on one edge to prevent rubbing. The angle of the thread will be maintained by the angle of the threading insert. Threading Operations.— There are many threading operations that can be programmed for a typical CNC lathe. Several operations require a special type of threading insert and some operations can only be programmed if the control system is equipped with special (optional) features: a) Constant lead single start threads (typically using G32 or G76) b) Variable lead threads—increasing or decreasing (special option) (G34 and G35) i) Multi-block threads (so called long-hand threading, block-by-block) (G32) The most common threading modes use either G32 (G33 on some controls) and G76. Threading Cycle (G32).— The G32 command is sometimes called “long-hand thread ing,” because each tool motion is programmed as one block. Programs using G32 can be quite long and virtually impossible to edit without major reprogramming. On the other hand, G32 method offers great flexibility and often is the only method that can be used, particularly for special threads. The programming format for G32 requires at least four blocks of input for a single thread pass from a start position: N__ G00 X__ Z__ N__ (G00) X__ Current threading pass diameter N__ G32 Z__ F__ Actual thread cutting (X__ Z__ for taper threads) N__ G00 X__ Retract to X-start position N__ Z__ Return to Z-start position Threading Cycle (G76).— G76 is a multiple repetitive cycle for threading, and is the most common method used to generate most of thread forms. Similar to roughing cycles, G76 is programmed in two versions, depending on the control system used. For older controls, a one-block format is used, for newer controls a two-block format is used. The two-block format offers additional settings that are not available in the one-block method. The G76 threading cycle requires information about the thread and the cutting method. One-Block Cycle: For a one-block G76 cycle, the format is: N__ G76 X__ Z__ I__ K__ D__ A__ (P__) F__ Where: X = the diameter of the last threading pass Z = the end of thread along the Z axis I = the amount of taper over the total length (per side) K = the single depth of the thread D = the depth of the first threading pass A = the included insert angle (only A0, A29, A30, A55, A60, and A80 allowed) P = the infeed method adjustment—positive (not available on all controls) F = the feed rate (thread lead) Two-Block Cycle: The two-block G76 format includes several additional programmable features that make the cycle more flexible. For a two-block G76 cycle, the format is: N__ G76 P__ Q__ R__ N__ G76 X__ Z__ R__ P__ Q__ F__ c) External and internal threading d) Tapered threads (conical threads) e) Right hand (R/H) and left hand (L/H) threads f) Face threads (scroll threads) g) Multi-start threads h) Circular threads (special option)
Copyright 2020, Industrial Press, Inc.
ebooks.industrialpress.com
Made with FlippingBook - Share PDF online