[magneto259]

Ok everybody I got it take my wpc. I had to put those coordinates in the G57 work offset screen. On my tool length offset all im offsetting is the length of the insert? Because it is a npt thread and i measure from the first tooth of the insert. Is that correct? Thanks in advance!!!!!!

[MDLang]

Your machine will default to the main programs wpc if you exclude the G57 or use a G54 instead.

If your parameters are set correctly you don't need an G43 and an H. If not include them.

Below is an example of a threadmilling sub that I can run from a Mazatrol main. I used diameter offsets only so I can pull two passes using the same programmed path with different offsets.

On a one pass program I omit the D address completely and let it default to the Mazatrol tool data. Again the parameters must be set correctly.

The G30 is second reference position or tool change position.

(3/4-14 NPT, .5 SHANK .495 DIAMETER 4 FLUTE )
(CARBIDE THREADMILL, RIGHT HAND INTERNAL THREADS)
(DIA = 1.0672 DEPTH = 0.5457 PITCH = 14)
(REMEMBER - PROGRAMMED CENTER LINE OF CUTTER)
(G41 CUTTER COMP, LARGER TOOL DIAMETER = SMALLER)
(THREAD DIAMETER, SMALLER TOOL DIAMETER = LARGER)
(THREAD DIAMETER, SHOULD FINISH CLOSE TO ZERO)

(TOOL POSITION FROM TOP/CENTER OF HOLE)
(X0.0 Y0.0 Z0.0)
(FIRST PASS, D08 DIAMETER OFFSET)
(.025 UNDERSIZE)

G20 G40 G80 G90 G95
G30 Z0.0
G30 X0.0 Y0.0
T08
M06
G00 X0.0 Y0.0 Z3.0 S1800 M03
Z0.0 M8
G91 G01 Z-.5546 F.06
G41 X.1514 Y-.1514 F.03 D08
G03 X.1514 Y.1514 Z.0089 I0.0 J.1514 F.002
X-.3028 Y.3034 Z.0179 I-.3028 J0.0 F.0035
X-.3039 Y-.3034 Z.0179 I0.0 J-.3034
X.3039 Y-.3045 Z.0179 I.3039 J0.0
X.3050 Y.3045 Z.0179 I0.0 J.3045
X-.1525 Y.1525 Z.0089 I-.1525 J0.0
G01 G40 X-.1525 Y-.1525 F.06
G00 Z.4654
G90 Z1.0

(SECOND PASS, D09 DIAMETER OFFSET)
(ON SIZE)

Z0.0
G91 G01 Z-.5546 F.06
G41 X.1514 Y-.1514 F.03 D09
G17 G03 X.1514 Y.1514 Z.0089 I0.0 J.1514 F.002
G03 X-.3028 Y.3034 Z.0179 I-.3028 J0.0 F.0035
X-.3039 Y-.3034 Z.0179 I0.0 J-.3034
X.3039 Y-.3045 Z.0179 I.3039 J0.0
X.3050 Y.3045 Z.0179 I0.0 J.3045
X-.1525 Y.1525 Z.0089 I-.1525 J0.0
G01 G40 X-.1525 Y-.1525 F.06
G00 Z.4654 M09
G90 Z3.0 M05
G30 Z0.0
G30 X0.0 Y0.0
M00

Mike

[magneto259]

Thanks for the input. I was going to try to do all the cutting in one pass. Is it better to do 2 passes? Thanks in advance!!!!!!

[MDLang]

It is suggesested that NPT holes are taper reamed after tap drilling.

A quick check puts the radial depth of cut for a 1.25-11.5 at around .07 over the 1.5 tap drill size and that may be a bit heavy for the teeth on the threadmill.

I don't have alot of experience with NPT threadmilling but I would hesitate to take it in one pass unless it has been reamed

Mike

[magneto259]

Yeah that is a good idea. Thanks!!!! I'll try a 2 passer when I get my hands on the machine.

[magneto259]

Well i tried it this morning and it picked up my X,Y coordinates that i put in the G57 but it completely blew off my Z coordinate and tried to bury the toolholder into the part???? So i took the part and fixture to do a dry run and the pallet came in all the way and softlimited out. Why would it disregard the Z coordinate i put in the G57 offset? Here is my code any help is appreciated!
Here is what i put in my G57 X-11.0233 Y-11.7676 Z-25.467
Thanks in advance!!!!!!

T2
M06
G94
G90 G00 G57 X0. Y0. T2
G43 H2 Z2. M3 S2772
G91 X0 Y0 Z-2.1035
G91 G01 G41 D60 X0.2623 Y-0.6597 F10.75
G91 G03 X0.6598 Y0.6597 Z0.0165 I0J0.6597 F10.75
G91 G03 X-0.2699 Y0.6522 Z0.0109 I-0.9222 J0.0004 F35.84
G91 G03 X-0.6522 Y0.2705 Z0.0109 I-0.6526 J-0.6521
G91 G03 X-0.6527 Y-0.2700 Z0.0109 I-0.0004 J-0.9229
G91 G03 X-0.2707 Y-0.6527 Z0.0108 I0.6525 J-0.6531
G91 G03 X0.2702 Y-0.6532 Z0.0109 I0.9236 J-0.0004
G91 G03 X0.6532 Y-0.2709 Z0.0109 I0.6536 J0.6530
G91 G03 X0.6537 Y0.2704 Z0.0108 I0.0004 J0.9243
G91 G03 X0.2711 Y0.6537 Z0.0109 I-0.6535 J0.6541
G91 G03 X-0.6598 Y0.6597 Z0.0165 I-0.6597 J0
G00 G40 X-0.2650 Y-0.6597 Z0
G91 X0 Y0 Z-0.1208
G91 G01 G41 D60 X0.2406 Y-0.7018 F11.09
G91 G03 X0.7019 Y0.7018 Z0.0171 I0J0.7018 F11.09
G91 G03 X-0.2758 Y0.6667 Z0.0109 I-0.9426 J0.0004 F36.98
G91 G03 X-0.6667 Y0.2764 Z0.0109 I-0.6671 J-0.6665
G91 G03 X-0.6671 Y-0.2760 Z0.0109 I-0.0004 J-0.9433
G91 G03 X-0.2767 Y-0.6671 Z0.0108 I0.6670 J-0.6676
G91 G03 X0.2762 Y-0.6676 Z0.0109 I0.9440 J-0.0004
G91 G03 X0.6676 Y-0.2769 Z0.0109 I0.6680 J0.6675
G91 G03 X0.6681 Y0.2764 Z0.0108 I0.0004 J0.9447
G91 G03 X0.2771 Y0.6681 Z0.0109 I-0.6679 J0.6685
G91 G03 X-0.7018 Y0.7018 Z0.0172 I-0.7018 J0
G00 G40 X-0.2434 Y-0.7018 Z0
G90 G00 Z6.0000 M52
G49 M5
M99

[tobyaxis]

T2
M06(Use M6, extra zeros take up valuable space in the memory)
G94(Feed Inches Per Minute, probibly don't need this because it is Modal at Machine start up AKA Power On)
G90 G00 G57 X0. Y0. T2(G0 and you don't need the T2 here)
G43 H2 Z2. M3 S2772(Spindle Speed and Rotation should be in the block after the G94 Block)
G91 X0 Y0 Z-2.1035(All these G91's aren't needed, G91 is Modal until G90 is Commanded)
G91 G01 G41 D60 X0.2623 Y-0.6597 F10.75(assuming that this Mazak has a lot of Tool Pockets D60 is fine as long as you designate the Radius of the Tool in the Offset Geometry Page)
G91 G03 X0.6598 Y0.6597 Z0.0165 I0J0.6597 F10.75(You only need one G3)
G91 G03 X-0.2699 Y0.6522 Z0.0109 I-0.9222 J0.0004 F35.84
G91 G03 X-0.6522 Y0.2705 Z0.0109 I-0.6526 J-0.6521
G91 G03 X-0.6527 Y-0.2700 Z0.0109 I-0.0004 J-0.9229
G91 G03 X-0.2707 Y-0.6527 Z0.0108 I0.6525 J-0.6531
G91 G03 X0.2702 Y-0.6532 Z0.0109 I0.9236 J-0.0004
G91 G03 X0.6532 Y-0.2709 Z0.0109 I0.6536 J0.6530
G91 G03 X0.6537 Y0.2704 Z0.0108 I0.0004 J0.9243
G91 G03 X0.2711 Y0.6537 Z0.0109 I-0.6535 J0.6541
G91 G03 X-0.6598 Y0.6597 Z0.0165 I-0.6597 J0
G00 G40 X-0.2650 Y-0.6597 Z0
G91 X0 Y0 Z-0.1208
G91 G01 G41 D60 X0.2406 Y-0.7018 F11.09
G91 G03 X0.7019 Y0.7018 Z0.0171 I0J0.7018 F11.09
G91 G03 X-0.2758 Y0.6667 Z0.0109 I-0.9426 J0.0004 F36.98
G91 G03 X-0.6667 Y0.2764 Z0.0109 I-0.6671 J-0.6665
G91 G03 X-0.6671 Y-0.2760 Z0.0109 I-0.0004 J-0.9433
G91 G03 X-0.2767 Y-0.6671 Z0.0108 I0.6670 J-0.6676
G91 G03 X0.2762 Y-0.6676 Z0.0109 I0.9440 J-0.0004
G91 G03 X0.6676 Y-0.2769 Z0.0109 I0.6680 J0.6675
G91 G03 X0.6681 Y0.2764 Z0.0108 I0.0004 J0.9447
G91 G03 X0.2771 Y0.6681 Z0.0109 I-0.6679 J0.6685
G91 G03 X-0.7018 Y0.7018 Z0.0172 I-0.7018 J0
G00 G40 X-0.2434 Y-0.7018 Z0
G90 G00 Z6.0000 M52
G49 M5
M99


Here is and Example of a .675-18 Thread Mill Program in one Swift Helical Movement.

O0001
G0G17G40G49G54G80G90M5
G91G28Z0M9
G90
M1

N1(THREAD MILL .675-18 ODD-BALL)
T1M6
G90G54G40G0X0Y0S650M3
G43Z1.0H1
Z.1M8
G1Z-.25F15.0
G41G1D21X.3375F8.0
G3I-.3375Z-.3055F36.1075
G40G1X0F60.0
G0Z.1M9
Z1.0M5
G91G28Z0M19
G49G90
M30
%

Nice Clean and Simple.

BTW: This is my first Thread Milling PGM.

Cheers!!!!!!!!:cheers:

[magneto259]

Ok i'll clean it up and see what happens on monday! Thanks

[tobyaxis]

Ok i'll clean it up and see what happens on monday! Thanks

I just hope that this helps you out.

Cheers!!!!!!!!!!:cheers:

[magneto259]

Trust me any little bit helps me...lol! Hopefully i can put in a machine and run it sometime. Its hard to get to a machine when we are running production.

[jackson]

Make sure your not going to deep with your initial Z- dive it is showing -2. something just make sure your drill is going deeper than that

[magneto259]

It is going not quite that deep. I thought it was taking the measurement off of the initial Z2. then going Z-2. from there.

[tobyaxis]

It is going not quite that deep. I thought it was taking the measurement off of the initial Z2. then going Z-2. from there.

Z0 should be the Top of the Part. Everything below that is Z-(minus)

[magneto259]

Hmmm.... i wonder why the vardex thread mill program spits that out when i specify the depth as .760?????

[tobyaxis]

Hmmm.... i wonder why the vardex thread mill program spits that out when i specify the depth as .760?????

If the Top (Highest Surface) is Z0 that Depth will be Z-.76. All of your tools should be touched off on the Probe then One tool to Teach the Z0 in the Setup Page.

[petek]

on my machine g28 z4 m5 would attempt to send the axis 4" above the machine 0 -not possable- try z0 or z-(something)

[magneto259]

Thats how i set my Z0 in my WPC is by touching off of the part surface and i understand everything after that is a -number. I was just curious as to why their program would spit out that odd number??? The weird thing is when i look at it in NCPLOT it only shows it going like -.1035 instead of -2.1035?????
Strange.........Thanks for the replys!!!! Thanks in advance!!!!

[magneto259]

Well I did a dry run and it works!!!! Here is the code i ended up using
T11
M6
G90 G57 G00 X0 Y0 S4210 M3
G43 Z1 H2
Z-.810 G41 X.4524 Y-0.099 D60
G03 X.551 Y0 Z-0.788 I0 J0.099 F35
Z-.701 I-0.551 J.0
X.4524 Y.099 Z-.679 I-0.099
G40 G00 X0 Y0
G28 Z.0 M05
M99

It looks good in NCplot and works in the machine but i still have to run a part with it. Maybe i'll get a chance to tomorrow. Thanks for all the help everyone!!!!!! I'll keep you posted.

[tobyaxis]

Thats how i set my Z0 in my WPC is by touching off of the part surface and i understand everything after that is a -number. I was just curious as to why their program would spit out that odd number??? The weird thing is when i look at it in NCPLOT it only shows it going like -.1035 instead of -2.1035?????
Strange.........Thanks for the replys!!!! Thanks in advance!!!!

NC Plot shows the Center Line of the Programmed Tool because you can't enter Radial Offset Cutter Compensation.

BTW: Congrats on your Success!!!!!!!!! :rainfro:

[magneto259]

Ok thanks i thought the lead in and lead out looked alittle wierd. But i'll see what happens when I run it in the machine. Thanks!!!!!!