|
View Full Version : Thread milling help! asjad 04-08-2007, 11:45 AM I want to make a programme for inside thread milling by interpolation method using single point thread milling cutter ...... how can i make programme for 28 mm inside core dia with 1 mm pitch in 25 mm depth........ If i have got dia 10 mm single point HSS cutting tool. Geof 04-08-2007, 02:49 PM This program has the Work Zero at the center of the hole and Z zero at the top of the material and it uses Tool Compensation which is entered by the G10 command. I have not accurately calculated the diameter for the thread so you would need to do that, I am just using 30mm to make it easy. Also this is just the thread milling part so you would need to interpolate the hole first. G10 L12 G90 P1 R10.0 Enter the tool diameter G00 X0. Y0. Z1. Move to the hole center Z-25.0 Move to the starting depth G41 D01 G01 Y10. F25. Set tool compensation but do not enter the cut yet G03 R12.5 Y-15. This does a halfcircle counterclockwise so the tool enters the cut tangentially and ends at a radius of 15mm G91 G03 I0. J15. Z1. L26 This does 26 circles incrementing up 1.0mm at each circle so the tool ends above the work G90 G40 Y0. Z1.0 This changes back to absolute, cancels tool compemsation and move clear of the work asjad 04-10-2007, 07:27 AM thanks you *Geof* i have made the same programme myself ... i wanted to know more techniqs..... anyway my job is done thanks again. dandy 04-10-2007, 01:47 PM try this website www.advent-threadmill.com/ I use their software for 90% of my thread milling dandy boxxer_boy 04-12-2007, 05:08 AM I know that one of our tool suppliers has a neat little porgram that you can download from there site.. the company is ISCAR. tturnbull50 09-21-2008, 11:47 AM try this I use it on fanuc O-M + 18 It is in metric but can be used for imperial as well T1 M6 G0G54X0Y0S2000M3 G43Z100.H1M8 M98P4000 G0X50. M98P4000 Z100. M30 :4000 (THREADMILL) #100 =-62.(START DEPTH) #101 =10. (RADIUS OF THREADMILL) #102 =42.(DIAMETER OF THREAD) #103 =150 (FEEDRATE) #104 =2.(THREAD PITCH) #105 =12.(TIP LENGTH) #102 =#102/2. #102 =#102-#101 WHILE[#100LT0]DO1 G1 G90 Z#100 F500 G1 G91 X#102 G3 G90 I-#102 Z[#100+#104 ] G01 G91 X-#102 #100 =[#100+#105+#104 ] END1 G0 G90 Z10. M99 |