1/8 NPT internal threeadmill

I am trying to do threadmilling on the lathe with live tools
Npt tap is in the centerline of the part
I was hopping there is some magic cycle which you run and puff part is with the thrad
No such a cycle
It is gildemeister sprint65 machine with 310 fanuc control
No Y axis on
So if i am not kistaken i need to engage somehow x,z,c and live tool to work together...

Is there some kind of magic trick to do it...
Never did it .ussually i either tap or single point.
This time in 316 matl tap is not working well....

So , please Help

The thread mill needs to move out in X while it is milling so that it ends up 1.7899 degrees from where it was in one pitch (1/27). You can divide the moves into quadrants. Feed thread mill into part, move X out to where you want to start milling, move C 90 degrees, Z 1/4 of the pitch and X 1/4 of where it needs to be to end up at 1.7899 degrees in one pitch simultaneously. Repeat this 3 more times to make a complete thread.

A) I don't think that many (most? any?) mills comp in D as they run the routine. I doo kind'a have a problem with this personally, but apparently not mechanically. You will never feel the change in PD at the apex of your thread doo to the fact that you are using a rotating cutter, unlike the 4 lines left by your tap.

I recently ran a 1" NPT and it was smooth as glass at the apex point, so I'm sure that you don't stand a chance of finding it on an 1/8 hole.

That said - I prolly would comp the U a bit if in a lathe - just b/c it is so simple to doo it and know that you made the best part that you could...

???


B) Programming it should be simple in a lathe.

M? ( Live tool on CW - opposite M code as the cross werking holder)
M? (C axis on)
G0 X0 Z.1 C0
G1 Z-?
X?
U.002 W.037 C(H?)-360.
G0 X0
Z1.


i SEE NO REASON TO GET QUADRANTS INVOLVED HERE. ??? (sorry - caps lock)


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

Think Snow Eh!
Ox

Without a Y axis I cannot conceive of a way this would work. Rotating C changes the angle to centerline. That blows your thread taper, thread angles etc

First of all
Thanks..
For some reason i did not think i can control all at once..C axis , X and Z while live tool is spinning..

It is working.
Tried with 4 quadrants
tried full C revolution

Both are working
Thanks guys

pgmrmike said:

Without a Y axis I cannot conceive of a way this would work. Rotating C changes the angle to centerline. That blows your thread taper, thread angles etc

Click to expand...

Well not really, Of course z is cutting inward and the thread taper form is built into the thread mill. So one is actually side milling. The only problem could be a parameter $etting. Or machine accuracy that may require a dummy move to minimize backlash. But the program is a solid basic approach and should actually be repeatable if you want/need to take 2 passes.

TeflonDave said:

Well not really, Of course z is cutting inward and the thread taper form is built into the thread mill. So one is actually side milling. The only problem could be a parameter $etting. Or machine accuracy that may require a dummy move to minimize backlash. But the program is a solid basic approach and should actually be repeatable if you want/need to take 2 passes.

Click to expand...

My bad, I misread the post, I didnt catch the part where you said it was at centerline and "assumed" you were trying to threadmill on the OD

I thread 1/4-18 all the time it works good for me here is a sample program using X,Z,C axis.

N70T1010(1/4-18 N.P.T. THREAD MILL)
(TOOL# 60020591)
M24
G99
G54.1P1
M8
S2315M33
G0X0Z.1C0
G98
G1Z-.6F50.
X.118Z-.5725H180.F2500.
Z-.5169H360.
X0Z-.4891H180.
G0X0C0
G1Z-.6F50.
X.168Z-.5725H180.F2500.
Z-.5169H360.
X0Z-.4891H180.
G0Z5.M9
G99
M35
#510=#510+1
IF[#510GE#610]GOTO5000
IF[#510LT#610]GOTO5001
N5000
#510=0
#3006=5(CHANGE THREAD MILL)
N5001
M1