I thread alot of stainlesss What kind of control are you using? What does DOC mean? I asume this is a lathe.1 1/4 dia. ,303 stainless
580 surface feet min.
580 x 3.82
/ 1.25= 1772 rpm that seem a little fast to me i would start at about 1000 rpm. Your leed will be .05 per rev. (1.00 / 20=.050 ) To find your thread height external. multiply leed x .61343 (.05 x .61343 = .0306) This is the height of the thread per side . So (.0306 x 2=.0612 ) 1.25 - .0612= 1.1888 this will be your final thread depth for x axis. To find the depth of thread for an internal thread mutiply thread leed x .54127 If you are using a Fanuc control your threading program might look like this depending witch model of control you have.This how I woud write it for a Fanuc
21T control
O1234 S 1000 M3 T0101 GO X 1.270 Z.1 M8 G76 P010160 Q0020 R.001 G76 X 1.1888 Z- 1.00 P0306 Q0050 F.050 M30
This program will cut an external 1.25 dia. 20 threads per inch ,1 inch long.
O1234( is just the program number ) S 1000 M3 ( the S calls for spindle, 1000 is rpm , M3 turns spindle on foward M4 is reverse. T0101 (T01 turns turret to tool 1 witch is going to be our threading tool the
01 is the tool off set . GO X 1.270 Z.1 ( GO is a rapid move the threading tool will travel at full speed to X1.270 and Z.1 this will place the threading tool a little above the shaft and .1 inch in front of the shaft M8 turns coolant on M9 coolant off
The G76 is a thread cuting cycle ,on a fanuc 21t control it uses 2 lines or 2 blocks ( a block is a single line of code) It will thread in at 29 deg.
1st block or line G76 P010160 Q0020 R.001 G76 call for threading cycle P010160 the first 2 digits 01 is number of spring passes or finishing cuts ,( Its just a pass with out moving the infeed in ,you can make 0 passes or up to 99 The thrid and forth digit is the thread let off
01 so on last thread it will gradully pull out so the thread just does not stop suddanly . If your threading up to a sholder and you want the nut to go as far as it can put 00 for the second and third digits this will suddanly stop the thread just before it hits the sholder. The forth and fith digits is the angle of the thread 60 is for a 60 deg.thread or 29 for a acme thread 29 deg. Q is the depth per pass radial, Q0020 this will feed the threading tool down .002 per pass or .004 dia. R is the infeend amount for last pass it feeds straght in insted or 29 deg. it just cleans the thread up.
Second G76 line G76 X 1.1888 Z- 1.0 P0306 Q0050 F.050 G76 call up thread cycle X 1.1888 is the depth of last cut Z-1.00 The thread is 1 inch long P0306 is the thread height .0306 inchs per side. Q0050 is the first threading pass. The first pass can be cut deeper. F.05 The f is for feed how far the thread advances per revolution , in this case 20 threads per inch 1inch /20 = .050 inch.
M30 end of program stop spindle turns coolant off returns to start or program.
The G76 threading cycle may seem complicated but its a lot easyer than writing it long hand it is a very powerfull caned cycle it took only 8 blocks (lines) and feed the threading tool in at 29 deg. If i could to write this program long hand and feed the tool in at 29 deg. it would take alot or figuring and alot of lines of code. And if i wanted to feed a little deeper all i have to change just 1 number. Hope this helps .