Machinery's Handbook, 31st Edition
CNC THREAD CUTTING
1377
Where the first block:
P = a six-digit data entry in three pairs: Digits 1 and 2—number of finishing cuts (01–99) Digits 3 and 4—number of leads for gradual pull-out (0.0–9.9 times lead), no decimal point used (00–99) Digits 5 and 6—angle of thread (00, 29, 30, 55, 60, 80 degrees only) Q = the minimum cutting depth (positive radial value—no decimal point) R = the fixed amount for finish allowance (decimal point allowed) Where the second block: X = the diameter of the last threading pass Z = the end of thread along the Z axis R = the amount of taper over the total length (per side) P = the single depth of the thread (positive radial value—no decimal point) Q = the depth of the first threading pass (positive radial value—no decimal point) F = the feed rate (thread lead) The P/Q/R addresses of the first block are not related to the P/Q/R addresses of the second block. They have their own meaning, applied within each block only. The G76 threading cycle is used to program the majority of CNC thread cutting opera tions. Several of parameters of the G76 cycle can be changed at the machine to optimize the threading operation. Example: The code block for cutting an external thread on 2 inch diameter, 12 threads per inch, using tool number 6 to the length of 1.5 inches (thread ends in a recess) would be: N31 T0600; N32 G97 S800 M03; N33 G00 X2.2 Z0.3 T0606 M08 (START POINT FOR THE THREAD); N34 G76 P010060 Q0040 R0.002; N35 G76 X1.8978 Z-1.5 R0 P0511 Q0100 F0.083333; N36 G00 X8.0 Z5.0 T0600; N37 M01; Multi-Start Threads.— Threads with more than one start can be programmed using either G32 or G76 threading commands. The lead (and feed rate) for multi-start threads is always the number of starts times the pitch. For example, a triple start thread with the pitch of 0.0625 (16 TPI) will be 0.1875 (F0.1875). In order to achieve proper distribution of each start around the cylinder, each thread has to start at an equal angle, determined by the following calculation: Thread cylindrical spacing angle = 360 / Number of starts To achieve this angular spacing, the Z-axis point for each start must be one pitch further than the previous start: Shift amount = Pitch Number of shifts = Number of starts − 1 Subprograms, Macros and Parametric Programming CNC programs use several techniques to allow the programmer to create complex pieces of code using CNC code building blocks. Subprograms.— Subprograms (also known as subroutines), are specially designed pro grams that can be called on demand by another program and repeated as desired. Such repetition can take place in one program or in several programs. The content of standard subprograms is fixed and can be used only for the intended, specific purpose. For variable type subprograms—called macros—a special control option is required (see page 1378). The main advantages of subprograms include transportability between programs (even machines), shorter programs, and easier editing. Any repetitive toolpath or machine activity is suitable to be developed as a subprogram.
Copyright 2020, Industrial Press, Inc.
ebooks.industrialpress.com
Made with FlippingBook - Share PDF online