Thread milling with live tooling

[jsimon]

We have a round part we a turning in a lathe. The part needs a bolt circle with 1/2-13 threads that need to be tapped very close to the bottom of the hole. Does anybody know how to program a thread milling cycle using the C and Z axis' on a bolt circle using live tooling in a lathe?

Similar Threads:

• C Axis Milling w/ Live tooling
• Anyone ever hear of "live tooling" or "dynamic live tooling" in verticle mills?
• Okuma LC20 With Milling/Live Tooling ???
• What is Live tooling versus "non-live tooling"?
• SL-20 live tooling

[rustyhunter]

We have a round part we a turning in a lathe. The part needs a bolt circle with 1/2-13 threads that need to be tapped very close to the bottom of the hole. Does anybody know how to program a thread milling cycle using the C and Z axis' on a bolt circle using live tooling in a lathe?

I know this is an old post and will be of no use to you now, but I found it whilst searching for a similar question. I have just made up a macro for fanuc controls to get around this problem. If anyone needs to thread mill on a a bolt circle with live tooling on a lathe then I'm sure the macro will help out. There is a macro for machinig diameters on a bolt circle and a macro for threading. Russ

[sinha_nsit]

Pl post the tested one if you are willing to share.

[RCaffin]

Dead easy in a mill of course.

Cheers
Roger

[rustyhunter]

Pl post the tested one if you are willing to share.

No problem, I am at work tonight and will try and tidy it up a bit then. It works as I have run it, but it's a work in progress. I will post when I get the chance.

[rustyhunter]

Sorry for the delay on this, completely forgot about it and remembered when I went back round to the lathes today. I'll post up what I have, it may be a bit rough compared to what some of the guys can do but it has worked great for me. I will post 3 different variations, first one is for creating holes using and endmill etc, second one is for threading using a single point tool such as the horn hobbing tools, and the 3rd one is for a single pass threading cycle for solid carbide endmills.


Create holes only. Good for making holes bigger to suit threads or for hole making in general.
%
O4567
(MACRO FOR C AND X AXIS B.C HOLES)


(CREATE DIAMETER WITH ENDMILL)


T0202
M41
(MAKE SURE CHUCK IS REFERENCED)
M13S800
G01C0F2.0
G52C0.(DATUM SHIFT TO SKIP HOLES)
G52 Z0. (DATUM SHIFT TO DETAIL FACE)


#502=14.5 (P.C.D)
#504=0.65 (DIAMETER OF CIRCLE TO CUT)
#506=.5905 (TOOL DIAMETER)
#523=0 (INITIAL C POINT, ALTER TO SUIT)
#524=6 (AMOUNT OF HOLES)
#531=-0.85 (DEPTH TO MILL CIRCLE)
#532=0.1 (MAX D.O.C)


(************************************************* ***********)
(DO NOT EDIT BELOW HERE)
#507=[#504-#506](amount tool needs to move to edge)
#508=[#502+#507](position of x edge of centre)
#509=1(degree of each turn to creat circle)
#510=[360/#509](amount of cuts)
#533=#531/#532(LOOPS)
#534=[ABS[#533]]
#535=[ROUND[#534]]
#537=#531/#535(ACTUAL D.O.C)
#536=#537

#520=[#507*[SIN[#509]]](Y MOVE FOR TRIANGLE)
#521=[#507*[COS[#509]]](X MOVE FOR TRIANGLE)

#515=[#502+#521]
#516=[#520/#515]
#517=[ATAN[#516]](C POSITION MOVE)

#518=#509
#522=1(COUNTER)
#525=360/#524
#526=1
(************************************************* ***********)


G01X#502F0.05
G01C#523F2.0
G00Z2.0
G01Z#537F0.02
F0.02
G01C#523
M98P4568L#535

WHILE[#526LT#524]DO2
#537=#536
G00Z1.0
#523=#523+#525
G52C#523
G01C0F2.0
G01Z#537F0.02
F0.02
M98P4568L#535
#526=#526+1
END2

G00Z10
M05
M00


M30



O4568(SUB FOR HOLES)
#522=1
G01Z[#537]
G01X#508F0.02

WHILE[#522LE#510]DO1


G01X#515C#517F0.02
#509=[#509+#518](COUNTER)

#520=[#507*[SIN[#509]]](Y MOVE FOR TRIANGLE)
#521=[#507*[COS[#509]]](X MOVE FOR TRIANGLE)

#515=[#502+#521](X POSITION MOVE)
#516=[#520/#515]
#517=[ATAN[#516]](C POSITION MOVE)
#522=#522+1
END1
#537=#537+#536
G01X#502
M99
%

Create thread with single point tool
%
O4569
(THREAD HOLES ON B.C WITH X AND C AXIS)


(SINGLE POINT HORN TOOL)


T0202
M41
(MAKE SURE CHUCK IS REFERENCED)
M13S1200
G01C0F2.0
G52C0.(DATUM SHIFT TO SKIP HOLES)
G52 Z0. (DATUM SHIFT TO DETAIL FACE)


#502=14.5 (P.C.D)
#504=0.765 (DIAMETER OF CIRCLE TO CUT)
#506=0.52 (TOOL DIAMETER)
#530=0.1 (THREAD PITCH)
#532=-0.8 (DEPTH TO CUT)
#524=6 (AMOUNT OF HOLES)
#523=0 (INITIAL C POINT, ALTER TO SUIT)


#509=1(DEGREE OF EACH TURN TO CREATE THREAD)
(************************************************* **)
(DO NOT EDIT BELOW HERE)
#534=#532/#530(NO OF CUTS)
#535=[ABS[#534]]
#536=[FUP[#535]](ROUND UP)
#537=#532
#507=[#504-#506](amount tool needs to move to edge)
#508=[#502+#507](position of x edge of centre)
#510=[360/#509](amount of cuts)
#531=#530/#510(EACH PITCH MOVE)

#520=[#507*[SIN[#509]]](Y MOVE FOR TRIANGLE)
#521=[#507*[COS[#509]]](X MOVE FOR TRIANGLE)
#515=[#502+#521]
#516=[#520/#515]
#517=[ATAN[#516]](C POSITION MOVE)
#518=#509
#522=1(COUNTER)
#525=360/#524
#526=1
(************************************************* *******)

G01X#502F0.05
G01C#523F2.0
G00Z2.0
G01Z#532F0.005
F0.02
G01C#523
M98P4570L#536
G01X#502

WHILE[#526LT#524]DO2
G00Z1.0
#532=#537
#523=#523+#525
G52C#523
G01C0F2.0
G01Z#532F0.02
F0.02
M98P4570L#536
G01X#502
#526=#526+1
END2

G00Z10
M05
M00
M30



O4570(SUB FOR SINGLE POINT THREAD)
#522=1
G01X#508C0F0.005


WHILE[#522LE#510]DO1

G01X#515C#517Z[#532+#531]F0.02
#509=[#509+#518](COUNTER)
#520=[#507*[SIN[#509]]](Y MOVE FOR TRIANGLE)
#521=[#507*[COS[#509]]](X MOVE FOR TRIANGLE)

#515=[#502+#521](X POSITION MOVE)
#516=[#520/#515]
#517=[ATAN[#516]](C POSITION MOVE)
#522=#522+1
#532=#532+#531(NEXT Z)


END1
M99


%


Create thread with single pass hobbing tool
%
O4571
(SINGLE PASS HOBBING X & C AXIS)


(SOLID CRABIDE HOBBING TOOL)


(ALTER #539 TO OPEN THREAD OUT)
(#539 WORKS AS TOOL OFFSET)
(1ST PASS #539=0.01 + CUTS TIGHT)
(2ND PASS #539=0.0)
(3RD PASS #539=-0.01 - OPENS THREAD UP)

T0202
M41
(MAKE SURE CHUCK IS REFERENCED)
M13S800
G01C0F2.0
G52C0.(DATUM SHIFT TO SKIP HOLES)
G52 Z0. (DATUM SHIFT TO DETAIL FACE)


#502=12.625 (P.C.D)
#524=24 (AMOUNT OF HOLES)
#530=0.0769 (PITCH)
#532=-0.95 (DEPTH)
#504=0.5 (THREAD DIAMETER)
#538=0.34 (TOOL DIAMETER)
#523=0 (INITIAL C POINT)
#509=1 (DEGREE OF EACH TURN TO CREATE THREAD)


#539=0.01(TOOL RADIUS OFFSET)
(#539=0.01 WILL HOLD TOOL -0.01 A SIDE)
(MINUS VALUE OPEN THREAD OUT)

(************************************************* ***)
(DO NOT EDIT BELOW HERE)
#506=#538+#539(TOOL CUT DIA)
#534=#532/#530(NO OF CUTS)
#535=[ABS[#534]]
#536=[FUP[#535]](ROUND UP)
#537=#532
#507=[#504-#506](amount tool needs to move to edge)
#508=[#502+#507](position of x edge of centre)
#510=[360/#509](amount of cuts)
#531=#530/#510(EACH PITCH MOVE)

#520=[#507*[SIN[#509]]](Y MOVE FOR TRIANGLE)
#521=[#507*[COS[#509]]](X MOVE FOR TRIANGLE)

#515=[#502+#521]
#516=[#520/#515]
#517=[ATAN[#516]](C POSITION MOVE)
#518=#509
#522=1(COUNTER)
#525=360/#524
#526=1
(************************************************* ******)

G01X#502F0.05
G01C#523F2.0
G00Z1.0
G01Z#532F0.02

F0.02
G01C#523
M98P4572
G01X#502


WHILE[#526LT#524]DO2
G00Z1.0
M01
M13
#532=#537
#523=#523+#525
G52C#523
G01C0F2.0
G01Z#532F0.02
F0.02
M98P4572
G01X#502
#526=#526+1
END2

G00Z10
M05
M30

M30


O4572(SINGLE PASS CARBIDE HOB)
#522=1
G01X#508C0F0.002
WHILE[#522LE#510]DO1


G01X#515C#517Z[#532+#531]F0.003
#509=[#509+#518](COUNTER)

#520=[#507*[SIN[#509]]](Y MOVE FOR TRIANGLE)
#521=[#507*[COS[#509]]](X MOVE FOR TRIANGLE)

#515=[#502+#521](X POSITION MOVE)
#516=[#520/#515]
#517=[ATAN[#516]](C POSITION MOVE)
#522=#522+1
#532=#532+#531(NEXT Z)


END1
M99
%


I only done this for myself on the machine so you can probably add quite a bit to it, looking at it there I would probably and in a variable for the feedrate for example. Hope this helps someone out. Russ

[rustyhunter]

I am just posting a slightly updated version for the PCD threading. I was going over a job and altered the macro to suit, it should make it a bit easier if anyone is needing it. I just used program number 1234 for the main program and 1235 for the sub, alter to suit yourself. I have also added in the drilling cycles to show the full program.Russ


O1234(PCD)
(PCD HOLES)
(Z DATUM IS DETAIL FACE)

(PROGRAM FOR SAMSUNG PL60 LATHE)
(DATE - 06-09-2017)
(TIME - 07:39)

N5G20G40G80G99
N10G28U0.
N15M05
N20M01

(12MM SPOT DRILL)
(DAB THREAD POSITIONS AND GET CHECKED.)
N25G20G18G40G99(WARNING - FEED PER REV SELECTED)
N30G28U0.
N35G00Z13.445
N40T0202
N45M41
N50M05
N55M45
N60M68
N65G28H0.
N70G00Z13.445
N75G00Z2.M08
N80G00C0.
N85G00X12.625
N90G97S1000M13
N95G83Z-0.05R-1.8F.005
N100C15.
N105C30.
N110C45.
N115C60.
N120C75.
N125C90.
N130C105.
N135C120.
N140C135.
N145C150.
N150C165.
N155C180.
N160C195.
N165C210.
N170C225.
N175C240.
N180C255.
N185C270.
N190C285.
N195C300.
N200C315.
N205C330.
N210C345.
N215G80
N220G00Z2.
N225G99
N230M09
N235G28U0.
N240G00Z13.445
N245M15
N250M05
N255M00


(10.8MM INSERT DRILL)
(## TOOL TO STICK OUT 2.9 ##)

(DRILL THREAD MINONR)
N260G20G18G40G99(WARNING - FEED PER REV SELECTED)
N265G28U0.
N270G00Z13.445
N275T0202
N280M41
N285M05
N290M45
N295M68
N300G28H0.
N305G00Z13.445
N310G00Z2.M08
N315G00C0.
N320G00X12.625
N325G97S1000M13
N330G83Z-1.45R-1.8F0.003
N335C15.
N340C30.
N345C45.
N350C60.
N355C75.
N360C90.
N365C105.
N370C120.
N375C135.
N380C150.
N385C165.
N390C180.
N395C195.
N400C210.
N405C225.
N410C240.
N415C255.
N420C270.
N425C285.
N430C300.
N435C315.
N440C330.
N445C345.
N450G80
N455G00Z3.5
N460G99
N465M09
N470G28U0.
N475G00Z13.445
N480M15
N485M05
N490M00



(16MM CHAMFER TOOL)
(TUNGALOY VSSD16L100S10 TOOL)

(CHAMFER THREAD)
N260G20G18G40G99(WARNING - FEED PER REV SELECTED)
N265G28U0.
N270G00Z13.445
N275T0202
N280M41
N285M05
N290M45
N295M68
N300G28H0.
N305G00Z13.445
N310G00Z2.M08
N315G00C0.
N320G00X12.625
N325G97S800M13
N330G83Z-0.185R-1.8F0.005
N335C15.
N340C30.
N345C45.
N350C60.
N355C75.
N360C90.
N365C105.
N370C120.
N375C135.
N380C150.
N385C165.
N390C180.
N395C195.
N400C210.
N405C225.
N410C240.
N415C255.
N420C270.
N425C285.
N430C300.
N435C315.
N440C330.
N445C345.
N450G80
N455G00Z3.5
N460G99
N465M09
N470G28U0.
N475G00Z13.445
N480M15
N485M05
N490M00


(THREAD HOLES)
(HORN TOOL M306)
(INSERT 306.6032.0519 AS45)
(TOOL TO STICK OUT 2.4 FROM COLLT)

(USE OPTIONAL STOP TO CHECK HOLES)

(USE #1 TO OPEN OUT THREAD)
(#1=-0.002 CUTS 0.002 TIGHTER)
(#1=0.002 OPENS UP THREAD 0.002)

(START HERE)
#1=-0.02(TOOL OFFSET)
(ALTER #1 TO OPEN THREAD OUT)
G28U0.
G00Z13.445
T0808
M41
M05
M45
M68
G28H0.
M13S1200
G01C0F2.0
G00Z2.0

#501=0.5(THREAD DIAMETER)
#502=12.625(P.C.D)
#506=0.3433(INSERT DIAMETER)
#530=0.07692(PITCH)
#532=-1.05(DEPTH)
#524=24(AMOUNT OF HOLES)
#538=0(AMOUNT OF HOLES DONE)

(####################)
(DO NOT EDIT BELOW)
#504=[#501+#1](OFFSET )
#523=0.0(INITIAL C POINT)
#534=#532/#530(NO OF CUTS)
#535=[ABS[#534]]
#536=[FUP[#535]](ROUND UP)
#537=#532
#507=[#504-#506](amount tool needs to move to edge)
#508=[#502+#507](position of x edge of centre)
#509=1(degree of each turn to create circle)
#510=[360/#509](amount of cuts)
#531=#530/#510(EACH PITCH MOVE)
#520=[#507*[SIN[#509]]](Y MOVE FOR TRIANGLE)
#521=[#507*[COS[#509]]](X MOVE FOR TRIANGLE)
#515=[#502+#521]
#516=[#520/#515]
#517=[ATAN[#516]](C POSITION MOVE)
#518=#509
#522=1(COUNTER)
#525=360/#524
#526=1+[#538]
(#####################)

G01X#502F0.05
G01C#523F2.0
G00Z1.
G01Z#532F0.005

F0.02
G01C#523
M98P1235L#536
G01X#502
G0Z2.

M01
M13

WHILE[#526LT#524]DO2
G00Z2.0
M01
M13
#532=#537
#523=#523+#525
G52C#523
G01C0F2.0
G01Z#532F0.02
F0.02
M98P1235L#536
G01X#502
#526=#526+1
END2
G00Z2.0
G28U0.
G00Z13.445
M15
M05
M00

M30


O1235(PCD SUB)
#522=1

G01X#508F0.005
WHILE[#522LE#510]DO1
G01X#515C#517Z[#532+#531]F0.02
#509=[#509+#518](COUNTER)

#520=[#507*[SIN[#509]]](Y MOVE FOR TRIANGLE)
#521=[#507*[COS[#509]]](X MOVE FOR TRIANGLE)

#515=[#502+#521](X POSITION MOVE)
#516=[#520/#515]
#517=[ATAN[#516]](C POSITION MOVE)

#522=#522+1
#532=#532+#531(NEXT Z)

END1
M99

[g-codeguy]

Came across this old thread while searching how to thread mill an NPT side port on a Doosan TT1800SY with a multi-form thread tool.

First let me mention that I've never programmed a mill....only lathes for almost 34 years. Therefore I am not familiar with thread milling. Company replaced several old lathes with Doosan lathes having a Y-axis. This is my first job requiring a thread milling operation. Tapping is not an option. Also G80 codes are something I've only needed to use a couple times (G83) as they weren't available on the lathes we had until a few years ago. Didn't 'need' obviously, but it shortened my programs. Always a plus.

Second I don't need a macro program at this time...but may in the future.

Third: Couple questions for rustyhunter. Seems like lot of repetition. Couldn't you use While statements for the Spot Drill, Drill and Chamfer operations? How about a subprogram? My preference would be to combine the two if possible. A subprogram with the G83 and C-codes, a While statement to index and use a G65 call to pass the Z R & F values to the G83. However, like I said, my knowledge of G80 codes is severely limited so I don't know (yet) what can be done with them.

Now on to my problem. I am making lead-in and lead-out arcs. The G3 code for the thread cut appears to be working correctly...I am running the tool in the air above the part. However, the lead-in/out arcs look to be going in the wrong direction. They are feeding out of the part instead of into it like the actual thread cutting pass. Sample I was given showed to lead-in and lead-out at 1/2 pitch. I am using U- values in all 3 blocks so it is stumping me why the tool goes in the plus direction. I do know on older Fanuc controls that if the arc endpoint is wrong, the turret will move in an arc until it reaches the programmed point if using a R resulting in something you weren't looking for. I'm thinking that is no longer what happens with the new Fanuc controls. I & K used and the control will alarm if programmed with the wrong endpoint.

Am making two 1/8-27 NPT thread ports. I want to use G41/G42 to control the thread size rather than having to modify the program. I was told when I first started programming lathes not to use G41/G42 because we had to be able to copy the programs for use in all our lathes. As you can probably guess the lathes were old when I started. So it is also something I am not familiar with. Can I be in the hole and program a G42 with the G3 lead-in arc without crashing the tool? Tool is .310 diameter, hole .339 diameter.

I just realized this morning that my sub routine did not make use of G42. Right now it looks like this:

X1.1358
G3U-.037W-.0466R.0466
U-.0741R.0932
U-.037W.0466R.0466
G0X1.8
M99

Thread root diameter at the outer edge of the part should be .4032 as laid out per the Machinery Handbook. I could change the W's to Z's but don't see how that would change anything. I am working with Doosan, but haven't solved the problem yet. Partial order has to be shipped in 2 days so I thought I'd try for some help here since I can't talk to Doosan on a Sunday. Thanks.

EDIT: rustyhunter...laid down for a short nap and it hit me that you could use a K in the G83 blocks to drill 24 equally spaced holes. No need for fancy statements or subprograms.

G83Z-.05R-1.8F.005K24.

Would have to look when I get to work tomorrow, but pretty sure this is correct. Wouldn't have remembered, but the first job we did on a new lathe a couple months ago happened to be a repeat of one of the only one or two jobs I ever programmed using G83.

[deadlykitten]

hi g-code, i have a helix soubroutine, inside which i can control a few things :
... lead-in & lead-out movements : perpendicular line, tangent line, arch
... full circle when cutting depth had been reached ( disabled for thread milling )
... feeding on Z+ or on Z- ( i disabled this function inside my latest code variant )
... radius
... phase ( good to create multi-point start threads, or to generate custom infeed patterns for single threads )
... paterning possibility, so to repeat entire operation among a segment, or among an arch
... others :
...... machine specs : rpm, feed, spindle sense, coolant, etc
...... in operation work : clearance position on demand

if you combine the 'phase & radius' with the 'paterning', and there are many threads to be cut, you will be able to rough them with one tool, and finish them with another

i am sorry, i don't have codes for doosans; i shared these hoping to show the real possibilities that are available with parametric codes

even if the operation is not on spindle center ( thus excentric), it can be executed without using the Y axis ( thus only with XC interpolation), but it may perform smoother if Y axis is used / kindly

[g-codeguy]

Sounds complicated. I've done a few Macro B programs, but nothing really tough. I enjoy that type of programming.

[deadlykitten]

Sounds complicated

yup, it may sound complicated, but is always possible to delete something from a complex code

i almost forget, there are 2 more things :
... feed calculation not on live-spindle(tool) center, but at tool periphery
... computing the overlapping segment, for example, if the thread is cut within a single helix revolution, then the tool should continue cutting a bit more, so to avoid the case where the lead-in arc and lead-out arc have common points; something like, when chamfering by interpolation, you don't move 360*, but 360*+[1-2mm overlapp]; if this is not done, then the go-gauge may not slip well; an alternative is to increase the diameter of the helix / kindly