thread mill help

[hacdlux]

trying to do some thread milling
(tried single point tut material is too stringy)
tool is in my endworking attachment
tsugami ss32 fanuc 31i

im getting a plane select error


M50
M01
(TOOL - 4 OFFSET - 12)
(THREAD MILL 6/32)
(.098 THREAD MILL)
G28 U0.
G0 T1212
G17
M50
G0 X0. Z-.25
C90.
G97 S2500 M224
Z-.1
G98 G1 Z-.100 F3.
X.04
G17G3W.03125R.02F.75
G3W.03125R.02
G3W.03125R.02
G3W.03125R.02
G3W.03125R.02
G3W.03125R.02
G3W.03125R.02
G3W.03125R.02
G3W.03125R.02
G3W.03125R.02
G3W.03125R.02
G3W.03125R.02
G3W.03125R.02
G1X0
Z-.200
G28 U0. H0. M25
M01
M225
M51
G18

[CitizenBrian]

When I do threadmilling from a live endworking tool I use the "C" axis not a full blown helical interpolation cycle. See below

(Citizen A32)
M180S5=2500
T3200(THREADMILL)(1/4-20)
G0X0Z-.1T32
G0C0.
G98G1Z.675F25.
/B4
X.06F2.
W-.05H-360.F1000.
W-.05H-360.
W-.05H-360.
W-.05H-360.
W-.05H-360.
W-.05H-360.
W-.05H-360.
W-.05H-360.
W-.05H-360.
W-.05H-360.
W-.05H-360.
W-.05H-360.
X0F25.
G0Z-.25T0

But as far as your alarm goes I would say select a different plane???

[hacdlux]

i normally prefer full helical because you lock the brake and get much more rigidity but its only a .050 shank cutter so why not

[hacdlux]

i normally prefer full helical because you lock the brake and get much more rigidity but its only a .050 shank cutter so why not

[hacdlux]

i figured it out

r is to ambiguous for helical you have to use ijk

replaced my r values with i and it worked

[petriej]

I would do a ZC as well. From a compatability standpoint it is more widely accepted. I'm not familiar with that tsugami, but with a star or citizen back working station it works the best. Comps are easily done in just X(or whatever your main cross axis is). Don't have to worry about cutter comp and making sure that you have enough entry/exit to avoid crc alarms.

Also some machines don't have polar or helical. If it has a c axis sub that's all you need.

Some companies call this ID whirling and making sure that the tool is on center/thread is on center becomes a non issue.

You could easily write this as a macro.

[hacdlux]

all my lathes are y axis and y2 in the tsugamis case.

only time i use c axis is od engraving

i have had a few instances where i needed to drill a round botom hole and used a ballnose endmill like a boring bar running the endmill and the spindle and interpolating the arc

[SirDenisNayland]

I'll agree with the others about ZC over XYZ..
One its one less axis to worry about, for both programming and interpolation 'errors' (whipping around a twenty thou arc leads to roundness issues)
Two its going to be dead nuts concentric since you're not interping around, and you're not relying on the tool being perfectly dialed, which in my opinion will never be "perfect"
Three, because of those interp problems you can 'push' the ZC a lot harder: the tool may deflect but that deflection is going to be constant, so its going to be perfectly centered and perfectly round.
Four, C moving or C locked, your going to be equally as rigid, you're in the guide bushing after all and relying on the C axis servo in both cases.

Then again its just a thread and the tolerances make up for any and all errors you may encounter, even if you can never measure them.

Just food for thought.

Cheers

[hacdlux]

i changed it to zc this morning,

set it up and got it adjusted and a trial part out,

hopefully tomorow i can get my other setups wrapped up and finish the setup on this one,