CNC REPETITIVE COMMAND RULES Machinery's Handbook, 31st Edition
1374
where: P__ = the first block number of the finishing profile, Q__ = the last block number of the finishing profile, F__ = the cutting feed rate per revolution, S__ = the spindle speed in ft/min or m/min (cutting speed).
In all the examples, the spindle speed or feed rate can be omitted in the cycle, if already active (declared previously).The program example for G70 will use the data from the roughing operation: N__ G70 P6 Q11 F0.01 S400 Basic Rules for G71, G73 Cycles: It is important to observe some general rules, in order to make the multiple repetitive safe and efficient. Here are some more important rules: a) Apply a tool nose radius offset before the stock removal cycle is called. b) Cancel the tool nose radius offset after the stock removal cycle is completed. c) Return motion to the start point is automatic and must not be programmed. d) The P block in G71 should not include the Z-axis value for cycle Type I. e) Change of direction is allowed only for Type II G71 cycle and along one axis only. f) Stock amount U is programmed on a diameter (U+ for turning, U- for boring.) g) The Feed Rate programmed between the P and Q points will be ignored during roughing. h) Multiple repetitive cycles can be optimized at the machine by changing one or more settings. G72 and G73 are programmed in a similar way. G74 and G75 are used much less frequently and have a simpler format. Thread Cutting on CNC Lathes The method of thread cutting on CNC lathes is called single point threading using an indexable threading insert. As a threading operation is both a cutting and a forming opera tion, the shape and size of the threading insert must correspond to the shape and size of the finished thread. By definition, a single point threading is a machining process of cutting a helical groove of a specific shape with a uniform advancement per spindle revolution. The uniformity of the thread is controlled by the programmed feed rate in feed rate per revolu tion. Feed rate for threading is always the lead of the thread, never the pitch. For single start threads, the lead and the pitch are identical. As single point threading is a multi-pass operation, the CNC system provides spindle synchronization for each threading pass. Depth of Thread Calculations.— Regardless of the threading method used, the depth of a thread will be required for various calculations. It can be calculated from these common formulas ( TPI is the number of threads per inch): External V-threads (60-degrees for metric or US customary units): (1) Internal V-threads (60-degrees for metric or US customary units): (2) Thread Pitch = the distance between two corresponding points of adjacent threads. (3) In metric drawings, the pitch is specified as part of the thread designation. . . TPI Pitch 0 61343 0 61343 Depth of Thread # = = . . TPI Pitch 0 54127 0 54127 Depth of Thread # = = Pitch TPI 1 =
Copyright 2020, Industrial Press, Inc.
ebooks.industrialpress.com
Made with FlippingBook - Share PDF online