Trapezoidal Threading

[JHECNC]

Hi Guys,

New to this site so I hope this is the correct place to put this.

I've just got a job in which needs an M30 x 6mm Pitch Trapezoidal Thread 200mm long and I'm wondering how to go about it.As this is the first time I've cut a Trapezoidal Thread,Could some one point me in the right direction....Would you use a G76,G92 or a G32 Cycle ?

Machines available T200 Tornado (OT-C) and Daewoo Puma 2000SY (18i-TB)

Thanks for looking

Martin

[Fred the thread]

Martin,
threading with full form inserts can cause vibration problems which can be impossible to overcome, especially when cutting small diameters at long threading lengths. Using canned cycles is never a good way to make any thread, as they never quite do what you want them to!
As you have Fanuc controls with G32, then you can 'generate' the thread profile by juxta-positioing the tool edge along the thread profile. An off-the-shelf grooving tool should be able to do this thread with no problems.
Programming is straightforward. I have a VB based bit of software that I can run it through for you, if you so wish.
Just tell me the actual dimensions of Major, effective and minor diameters and thread spec and tolerance - i.e. TR DIN103 7e/7H The material, control system, maximum Z axis slide velocity and I will do the rest. I can even tell you which tool and insert you'll need.
Also, what is configuration of component? E.g. bar through bar-feed, billet.
How is component held? - Chuck soft jaws or hard jaws - or collet?
What tool shank cross section can your machine hold?
kindest
Fred the thread

[JHECNC]

Fred

Thanks for your reply.The Customers Dwg is a bit Vague,all it says is 30 x 6 Trapezoidal Thread,We are working to ISO 2904:1977.(Information here)

http://www.roymech.co.uk/Useful_Tabl...apezoidal.html

I have the inserts and tools.
Control is Fanuc OT-C and material is EN8 held between collet and tailstock.Maximum slide velocity is 6m/min.Although I will need to run it fairly slow as the amount of lead before the start of the thread is limited due to interference with the tailstock.I have run a couple of shorter testers using G76 and looks to be OK but the depth of each pass is 0.020mm

Martin

[Fred the thread]

Hi again Martin,
thanks for the link to the trapezoidal threads, it is most helpful.
There are a couple of problems you may encounter when using full form inserts and only going slowly as you put it with EN8, when cutting a thread 30mm dia. and 200mm long
They are a dull, torn surface finish due to insufficient heat at cutting edge and poor tool life / dimensional stability.
Full form inserts will not help, as the insert contact length will increase as it goes deeper into the component, giving increase in cutting forces, while the actual cutting speed (because of G97 constant rpm) will become less and less as the diameter reduces. Once you get vibrations, they are difficult to eliminate as the speed cannot be changed because the tool will not pick the thread up in the same place (scrap part) .
G32 allows two or more threading movements (but the control treats them as one movement remaining in pitch throughout) to enable the tool to accelerate into pitch, well clear of tailstock, then plunge to the programmed cut size after passing the obstruction and before engaging workpiece. If you have a Fanuc user's manual, look for G32 threading function and you will see a diagram and explanation for it. If you don't have a manual, let me know as I can send you a copy of the page.
G32 will also let you program a grooving tool which could be a more sympathetic way of doing this, as the (smaller) contact length on the insert will never change as the tool goes deeper into the thread, the cutting forces are much, much lower, and the inserts are usually less to buy - they will cover a large range of threads and pitches / threads per inch and they will also groove!
This is a well used trick in threading, especially when components are long and slender or thread form is large. It will let you run this thread of 30mm dia. at approaching 1,666 rpm - wow! that's nearly 158 metres per minute cutting speed at the major diameter! For this material 220 - 250 metres per minute would be better., but the restriction is 10,000 mm per minute slide velocity, so 1,666 rpm max it is.
By the way, we were cutting 200mm diameter 45mm pitch Stub Acme earlier this week on the end of a 3 metre long EN24T shaft using grooving style tool and insert with G32 and it went very well, good finish, correct size, just shut the door, press go and ... perfect thread, right to gauge first time, every time.
Another thing to check carefully is that the shim (sometimes called an anvil) under the insert presents the form at the correct helix angle - in order to balance the clearances and the cutting forces on both sides of the form. By my calculation, you going need 4 degrees, and 15 degree thread flank angles will not let you use anything more than a degree and a half away from that without serious rubbing on the insert below the cutting edge.
Tried to be as constructive as possible within your restrictions, sorry to have gone on a bit, but threading is my life.
I thread, therefore I am.
When do you expect to start machining the threads?
If you need more, let me know, the offer of a part-program if you want to use a grooving tool still stands.
kindest regards
Fred the thread

[JHECNC]

Fred

Thanks for the offer and all the info,very helpful.I was getting a bit frustrated with it so ended up staying one night to get it done.Did a couple of trial runs and ended up doing a G76 cycle plunging in 0.02mm depth of cut at 300RPM.(G76 P020000).
On my trial I did find that the Anvil was OK but the toolholder just rubbed on the last 2 cuts so that came out for filing.
It all worked out in the end so thanks for your help,I know who to call on for next time

Thanks

Martin