Thread Milling

I just wanted to know if anybody out there has thread mill on a M32 citizen on the sub. without having Y axis on the turret? I know it sounds like it would be able to, using X, Z, and C axis. But has somebody actually done it. Thanks

THIS IS A PROGRAM I RAN TO THREAD MILL A 3/8-16 THREAD IN A STAR SV-32 MACHINE.The "y" in this program is like "x" in most machines.

N5(ID THREAD-3/8-16)
G98M8(C-AXIS ON / IN. PER MIN.)
G0C0.
T2064(ID THREAD MILL)
#124=0.50(Z-DEAPTH)
#125=[#124/.0625*360]
G97
M47S1000(LIVE TOOL ON)
G0Y0.0T64
G0Z-0.10
G0Y0.145
G1W0.50H-#125F2000.
G0Y0.0
G0Z-0.10
G28V0W0T0
M48
M9
G99
M1

With all due respects to all responses, it kind of looks as if the above program is a hard numbered program for a thread whirl instead of a thread mill. That looks like our G32 for taps and screws where the H axis is our degrees in C. Thread milling should move in an actual Y axis. Otherwise I think your degrees that the C axis moves will make the thread "cave in" on itself. The more it moves in C one way, the closer your major diameter comes to touching itself. If you make a hole in G16, The hole is not round as it is eggshaped.

This is the way I have thread milled alot of parts using a single form thread mill. It seems to work real well. The threads look good and the thread gages work fine.

On an ID thread?

how are you setting your helical angle?

Thank you for the replys, ok i have read all of your replys but here goes a nother question. Same question as above but the thread being off center. I have a friend that is trying to thread mill an off center hole just using X,Z, and C axis. Can that be done and has somebody actually done it. The machine makes the movements but it is leaving a 2 flats on the major of the threads.

sorry i meant to write minor not major, sorry

Remember, you must take in to account the helical angle like whirling. The formula for that is tan-1[pitch/[pitchø*pi]]. Your flat is probably being caused by that. You still can not properly threadmill with out a proper Y axis or a tool that can be positioned at an angled other than 0/90

It might be in good interest to remember that thread mills are expensive. The average cost i hear is 100. Taps are much cheaper.

When the program posts it looks like this.

G0 G90 Z1.
G0 X.19 C_V$WSP$=180.000
G0 Z.1 F0.002
G1 Z0.
G0 G90 Z-.5206
G0 X.19 C_V$WSP$=180.000
TRANSMIT_S_V$WSP$
G0 X-.19 Y0.
G1 Z-.56
G1 G41 X.2475 Y0.
G3 X.2475 Y0. Z-.51 I-.4375 J0.
G3 X.2475 Y0. Z-.46 I-.4375 J0.
G3 X.2475 Y0. Z-.41 I-.4375 J0.
G3 X.2475 Y0. Z-.36 I-.4375 J0.
G1 G40 X-.19 Y0.
G0 Z.0394
G1 X-.1691 Z1.

M_V$WSP$13
TRANS_OFF
M_V$SP$=5
L_V$COFF$
G18 G40
VERSCHIEBUNG("OFF")
M_V$K$09 M_V$K$55
L710(1)
NN9999: M17

Here is a screen capture of what it looks like the attachment.

NOTE!!!!
DO NOT use a "Y" axis command for your turret unless you enter milling interpolation FIRST or you could damage the index mechanism. Even "Y0" will do this unless you have the newest version of software in the control.
Been there, Done that and paid dearly!

I am still confused why you would need a y-axis and why the helical is a problem. When you rotate c-axis that is just like moving x and y in a mill.
When you are thread milling in a mill your tool is not positioned on an angle.I have thread milled several parts in a star machine using c-axis and the parts looked fine and checked fine.

SWISS-TECH is correct you do NOT need to have the "Y" axis to threadmill. The tool would be made with all the angles in it either way. Somebody seems to be confusing Thread Whirling with thread milling.

Thank you for the replys, ok i have read all of your replys but here goes a nother question. Same question as above but the thread being off center. I have a friend that is trying to thread mill an off center hole just using X,Z, and C axis. Can that be done and has somebody actually done it. The machine makes the movements but it is leaving a 2 flats on the major of the threads.

the simple answer to your question is "Yes" but you need CAD/CAM to generate the toolpath/will take you forever to convert Y coord to angle.

You will NOT need to convert the "Y" axis commands yourself when using the Milling interpolation option. The control will do the work for you. (G12.1)

I know that G12.1 will convert C to Y axis. But will it work on a off center hole? I know the turret will over travel. But if it didnt over travel will it still work. Having X,C, and Z working together on a offset hole? G12.1 works good on X and C "Y" but how about all 3 axis.

yes, you need to order option 3 axis move to do XCZ move.

Yes, I have done it, exactly what you're referring to...
thread milling
internal thread
off-center
using the turret
on the sub
of an M-32
without a true Y-axis.

And here's the helpful part...
It was five years ago, and I don't have a copy of the program. (previous employer)

22-13-5 stainless was hard on taps, it milled much easier.
And we were making small pressure fittings, so threads without flats/scallops was essential.

iirc, it was pretty straightforward...
rapid to cl of hole
lock spindle in milling mode
rapid to (depth - 1 thread)
helix move to majorØ over a Z length of 1/2 thread lead (Important, to keep the thread crest from getting truncated)
helix move to depth
helix move out to cl of hole.

That being said, your code looks very strange to me:
M_V$WSP$13
TRANS_OFF
If this is what is posted, does it actually work?

My apologies for not having the code handy... it was literally 5 years ago, and I haven't laid hands on a CinCom program for at least three.
But half the battle is knowing it can be accomplished, yes?

I will look through my notes from back then and see if I can find something a little more helpful...

That code will look strange to you ghyman cause its not for a citizen, its for a DMG Gildemeister twin 65 machine. My friend is trying to do it on thier. I just figure if the citizen can do it that machine should be able to do it. I want to thank everybody for their input.

Been There And seen that As well....To elaborate on what Cogsman was justs saying....On M32's with out a Y2 Axis more than a couple years old....Y2 is actually TI...If you try calling a Y command when not in milling interpolation the control will take a Y command but will try to move the TI axis to where ever you told it...with the Turret still clamped....if you lucky TI will overload before any damage is done...but not ussually the Case..this shouldn't be the case on any newer M-32's I believe this has been addressed by Citizen...

threadmilling with CZ is cake

RAPID TO C0 Z-(CLEARANCE) AND X0
FEED INTO THREAD FULL DEPTH
FEED INTO WALL AT LOW FEED (MAJOR-TOOL DIAMETER) F~1.0
W-(2*PITCH) H-720.. (SPIN TWICE )
RAPID TO X0
GET OUT OF HOLE

WORKS GREAT, BEEN USING IT FOR YEARS, THE GREAT PART IS THE X OFFSET SETS THREAD DIA, DON'T HAVE TO MESS WITH THE R OFFSET

Swiss-Tech is using a live thread mill as a single point boring bar, but using inch per minute and one C rotation per pitch in Z(incremental). this works great on center. Thread mills may be expensive but I have got over 40,000 full thread form parts off one mill in Titanium using this method(4-40,2-56,0-80). Different parts require multiple methods. Also You can use G32 if your machine Spindle can be commanded low enough to get the proper surface footage(G32 taper off on the hypotenuse). Off or on Center I tend to start in mill interp(G12.1) much like the program posted.