Need Help!- Need help with thread milling program

[Lukema]

I am thread milling an M24 x 1 thread in cast iron. below is the sub program for the thread milling process. This sub program was writen years ago and the programer has since retired. I am having trouble following the sub program line by line. The machining center is a Deckel Maho Horizontal with a siemens 840D control.

;%_N_L921_SPF
;$PATH=/_N_SPF_DIR
;PROGRAM FOR DMG 1-8
;THREAD MILL CYCLE
;R2=REFERENCE DEPTH
;R3=FINAL DEPTH
;R5=PITCH OF THREAD
;R6=START OF THREAD RADIUS THAT IS SMALLER THEN TAP DRILL RADIUS
;R7=FINISH THREAD RADIUS
;R10=ADDITIONAL RETRACTION
N0010 G0 G60 G90 CFC Z=R2
N0020 R56=R7+R6 R57=R5/2 R62=-R6 R63=R56/2 R64=-R56
N0030 G0 G90 Z=R3
N0040 G1 G41 G91 X0. Y=R62
N0050 G3 G64 G91 X0. Y=R56 Z=R57 I0. J=R63
N0060 G3 G64 G91 X0. Y0. Z=R5 I0. J=-R7
N0070 G3 G64 G91 X0. Y=R64 Z=R57 I0. J=-R63
N0080 G0 G40 G60 G91 X0. Y=R6
N0090 G0 G90 Z=R10
N0100 M17

Parameters used, (all values below are in millimeters):
R56=22
R52=-10
R63=11
R5=1
R7=12
R64=-22
R6=10
R57=0.5

I am getting lost at line 60, how are the I & J being calculated?

Thanks for the help

[tfisher]

looks like a nice little program. the i and j in line 60 are the way they are because it looks like the program will move down to the minor radius as programmed in R6 then ramp in to the major radius as programmed in R7 since your tool is now at the major radius. line 60 will now make a complete circle rotating around the center of the hole which is -R7. I hope this will help if not let me know i can give it another try. If you are interested i have alot of nice macros for the siemens 840d. like thread milling pipe threads and boring a spherical bore. They told me it couldn't be done with the 840d but i got it to work and it works very well.

[Lukema]

Thanks tfisher,
So the x & y coordinates represent the end points of the arc and the I & J represent the are center?

The way i read it, the first move is Y-10
next is an arc starting at x0 y-10 and ending x0 y22 with the center of the arc being x0 y11.
This arc of 180degrees
what i am not getting is (-10) to 22 is a linear distance of 32mm, half of 32 is 16, so why is J=11 and not 16?

Next In line 60, is the end point of the arc actually x0 & y0, which would be the center of the bore,(no longer cutting)?
Is this line commanding a 180 or 360degree arc?

Then in line 70, end point of this arc segment is x0 y-22 with arc center at x0 y-11.
why is the end point of the arc x0 y-22 ? i would think x0 y-12 because of the thread having a major diameter of 24mm.

what am i missing here

Thanks for the help, this is driving me nuts
Luke

[tfisher]

i think what is messing you up is that you have to remember that G91 is active so all your coordinates are incremental. so you move to y-10 then do a 180 degree arc to y22 which is incremental so you are at y12 in absolute. that is why in line 60 your j is at -12 because you are at y12 in absolute coordinates. whenever using G2 or G3 your x and y dimensions can be absolute or incremental depending on whether you're using G90 or G91 but your i and j dimensions are always incremental. hope this helps.

[Lukema]

Thanks,

I got it now, I was thinking absolute and not incremental.

Thanks again for the help.
Luke