calling the lathe gurus..... I think its a fanuc g112 question...

WILLEO6709 · Oct 30, 2014

so I have this part I run, 8620 case hardened, masked for case and then later od ground and id threaded/ id finish bored in a final program. The problem is the thread,, there is a bloody index pin hole and the single point threading bars I have get their tips whupped off a little too often, I spend more time screwing with offsets than running that op. so I get a seemingly bright idea... this machine has live tools... threadmill it.
The only problem is I have never used the "polar coordinate interpolation" feature. It all starts good but its going about +1000 times the x movement and -1000 times C axis movement....

as far as thread bars I have tried, Kennametal lt11 laydowns in kc5025, Iscar laydown in IC908, Its a 0.740 min bore with a 16 pitch un.... min 3/4 depth....

Has anybody ever driven a theadmill down the z axis instead of a thread bar? or do I just need some different grade in a multi tooth insert?

Machine is a TC-2L amera seiki from 1996 with a 0-TC, live tools, s20 collet.....

Hertz · Oct 30, 2014

Very much possible. Was just discussed actually in this thread http://www.practicalmachinist.com/vb/cnc-machining/thread-milling-live-tooling-293312/

WILLEO6709 · Oct 30, 2014

T0101
G98
M43
G97S1000M13
G0C0.
G0Z.25
G0X1.5
G112
G1X0.C.75F500.
Z.1
Z-.5F25.
C.7075F5.
G3X.0336Z-.4976C.7043R.0457
X.125Z-.4875C.75R.0457
X0.Z-.475C.8125R.0625
X-.125Z-.4625C.75R.0625
X0.Z-.45C.6875R.0625
X.125Z-.4375C.75R.0625
X.0336Z-.4274C.7957R.0457
X0.Z-.425C.7925R.0457
G1C.75
Z-.25F25.
C.7075F5.
G3X.0336Z-.2476C.7043R.0457
X.125Z-.2375C.75R.0457
X0.Z-.225C.8125R.0625
X-.125Z-.2125C.75R.0625
X0.Z-.2C.6875R.0625
X.125Z-.1875C.75R.0625
X.0336Z-.1774C.7957R.0457
X0.Z-.175C.7925R.0457
G1C.75
Z.1F500.
Z.25F500.
G113
G28U0.H0.M15
G28W0.

ok, the above example.... what are the C values programmed in? Its surely not degrees
do I need to call out a G17 or is that assumed on the g112?
feedrates are calculated how?

WILLEO6709 · Oct 30, 2014

so why does this have to be so hard? If I can have both the main spindle running and the live tool can I just use a G76 cycle if the thread is on the center of the main spindle?

Hertz · Oct 30, 2014

The c outputs are not degrees when using G112. They are however when not using it. Taken from a manual. Go to page 24 of this link. It explains how it works with G112. http://www.productivity.com/content/customer/docs/HaasLiveToolOpProgram_w_DS Manual.pdf

Now as for threading on center, if you can, why not just use a tap?
You do not need the live tool.
Or if you want to use the live tool, then you would simply lock the c axis and run a thread live tool tap command.
As for using a thread mill, I've never used one in the same way a threading bar would be used so I can't even say anything about it but I'm pretty certain it will not work, lol.

I use software to program my c axis so I don't run into these issues. If you have software, use it. Good luck. HTH

yardbird · Oct 30, 2014

WILLEO6709 said:
If I can have both the main spindle running and the live tool can I just use a G76 cycle if the thread is on the center of the main spindle?

I don't have live tools so no help here. ^^^^ I would try that. I can't think of why this wont result in the desired thread. Seems you'd want a slower main spindle speed then you would for a single tip stationary bar. Out in the air of course.

Brent

yardbird · Oct 30, 2014

I don't know if the thread mills are designed to cut on both side of the tool or not, might have to change infeed angle of the G76 to plunge straight in. Just thinking out loud.

Brent

Ox · Oct 30, 2014

A) I aint never tried it (yet) ** but I don't see why this is difficult?
I would think that you could:

M203 S1500
G0 X0 Z.1
Z-.8
G1 X.15 (or whatever gets you to thread size)
M23 (C AXIS - WHATEVER YOUR CONTROL USES)
Z.1 H-(however many degrees for your pitch) F_*

Does it need to be harder than this? :scratchchin:

B) I have battled this in a similar app for yrs, and have finally gotten a setup that does good for me.
I chase the thread, then doo my "interuption work" and then go back and take a clean-up pass with the threading tool again.
It takes all of about 5 (7?) seconds extra and I get a WHOLE lot better results.

This and I am using NT2FL - 5025's - but it's in 1215 - although I like the 5025 in 8620 too I think... ???

*Actually - that is prolly H+ (plus) (or G91 C?)

** or have I? It seems like I've done something similar as this... ??? :scratchchin:

You may want to toss a C axis HOME command in there ... I was just high-lighting of course...

------------

Think Snow Eh!
Ox

angelw · Oct 31, 2014

Ox said:
A) I aint never tried it (yet) ** but I don't see why this is difficult?
I would think that you could:

Think Snow Eh!
Ox

Hi Ox,
Its as simple as you've suggested. Using Polar may be an issue if the control doesn't support Helical Milling with the C axis. If Polar is used the programmed path would be a Circular Interpolation move combined with a Z move, the same as when helical milling in X,Y and Z. The command line in Polar, after the Cutter is positioned to the correct Depth in X, would be as follows:

G03 (G02) I-# # J0.0 Z_ _ F? ?

Where
# # = distance from cutter centre, to centre of workpiece
_ _ = Lead of Thread

The simplest method is as how you have described, unless one knows for sure that helical is supported with C.

For the most part the program would be an incremental 360 deg move in C for each thread Lead. The final C move may have to be calculated depending on where the Thread finished.

Regards,

Bill

WILLEO6709 · Oct 31, 2014

I'm gonna need somebody to hold my beer.... I am gonna try the g76 route..... It looks good in dry trial....

Ox · Oct 31, 2014

With a live toy?

Depending on your RPM and # of passes - I would think that you could end up with a version of "Internal Polygoning".

--------------------

Think Snow Eh!
Ox

Hertz · Oct 31, 2014

WILLEO6709 said:
I'm gonna need somebody to hold my beer.... I am gonna try the g76 route..... It looks good in dry trial....

Interesting to hear how it goes. Good luck.

Ox · Oct 31, 2014

Also concerned that this approach may yield an excessively high feedrate situation as well - again - depending on what R's you're using...

-----------------

Think Snow Eh!
Ox

Orange Vise · Oct 31, 2014

If I'm reading your post correctly, your threaded hole is on spindle center so you don't want to use polar coordinate interpolation. The previous discussion was for a bolt circle offset from the center.

I'm not sure if your machine will let you use G76 with the live tool spinning as I've never tried it. I wouldn't recommend it anyway because the "right" way to do it is dead simple. Do it the same way you'd do it on a mill - plunge in, lead in, helix out, lead out, retract - except on a C-axis lathe, the helix part of your code ends up being 1 block:

G98 G1 Z__ H___ F___;

H is the incremental number of degrees. 10TPI over 1 inch = 3600 degrees. For climb milling on the main spindle, it should be a negative number, so H-3600.

F is in degrees per minute. Careful, because any subsequent line that doesn't have an H value will be fed in inches per minute.

pcasanova · Oct 31, 2014

I did a part where I used a threadmill and positioned the x that set the od of the thread then did
a g33 single pass at depth

G95 S100 M4
S3=3000
M3=4
M71
G0 X.085 Z.2 M8;initial position
M1=24
G33 X.085 Z-.4 K.0417
G0 X0
Z.2
S3=5
M3=05
M5 M9

WILLEO6709 · Oct 31, 2014

Orange Vise said:
I'm not sure if your machine will let you use G76 with the live tool spinning as I've never tried it.

I did a dry trial...... put an endmill in a live toy.... way out in front of the chuck... both live and main running + executing g76 works... at least on my machine.

Ox · Oct 31, 2014

Well come on with it!

I know there is only 8 oz left anymore, but standing here holding this is getting old!

-------------------

Think Snow Eh!
Ox

WILLEO6709 · Oct 31, 2014

Collet just arrived, had a threeadmill that should work, probably try it out saturday or sunday.....

Ox · Oct 31, 2014

Well YOU hold your own beer then! :argue:

------------------

Think Snow Eh!
Ox

yardbird · Oct 31, 2014

Ox, Hertz, Orange Vice,

If I had a lathe with live tools just for shits and giggles I'd see if my machine would do this without puking out a alarm. Wondering if any of you have tried on yours?

Brent

calling the lathe gurus..... I think its a fanuc g112 question...

Diamond

Stainless

Diamond

Diamond

Stainless

Titanium

Titanium

Diamond

Diamond

Diamond

Diamond

Stainless

Diamond

Titanium

Hot Rolled

Diamond

Diamond

Diamond

Diamond

Titanium

Similar threads