3 Pitch Acme Threading Help

[metx]

I have an oilfield threaded flangewe are machining that is killing me on the 4-1/8" 3 pitch external rh acme thread. I tried running with a 54 series on edge insert but about 3/4 way into the thread the insert shatters. 3 inserts later and it took my tool out with it.I think the helix angle of the thread is whats doing it. I have ordered a Sandvik laydown holder and inserts for this to try. The tech guy @ Sandvik told me to not use tangental infeed but feed straight in and to run at 300 rpm. This just seems fast to me for such a large thread. Has anyone here cut this size acme and lend some thoughts?
TIA,
Keith

[Geof]

I have not cut a thread like that but I have heard of angled insert supports that are intended to tilt the insert so it matches the helix angle. Sorry I can't give you any definite leads but you could ask your tooling supplier.

[Fred the thread]

Hi Keith,
there is another way....
thread profile generation!
It gets away from form tools and allows reasonable cutting speeds coupled with reduced insert / workpiece contact lengths.
You need a CNC control capable of G32 (or the manufacturer's equivalent).
That is the function that makes one threading pass per 4 lines of part-program.
You use very a stable grooving system such as Seco MDT (Multi-Directional Turning) and program points around the thread profile, with successive passes that do not increase in contact length.
The part-programming is very straightforward - I will generate a part-program for you, and tell you which toolholder / insert to use.
Let me know:-
External or internal thread
Major diameter (mid-tolerance size)
Minor diameter (mid-tolerance size)
Effective diameter (mid-tolerance size)
Actual thread pitch (or threads per inch)
Leading flank angle (14.5 degrees for Acme)
Trailing flank angle (14.5 degrees for Acme)
Length of thread
Undercut or wash-out at end of thread
Start position of thread (component front face position in Z axis)
Whether parallel or taper (if taper, taper per foot per side)
Whether part-program output should be inch or millimetres
Diameter or radius programming (e.g. if turning 5" diameter, do you write X5.0 or X2.5 in part-program?)
Style of lathe (flat bed front turret or slant bed rear turret)
Control system and model (e.g. Fanuc 0T)
Cross section of toolholder (e.g. 1" square or 32mm x 25mm)
Usable rpms available in machine (safe for component and set-up)
Maximum Z axis slide velocity maintaining pitch accuracy
Material to to threaded

This has proven many times to be far superior to full form threading.
Threads with pitches of 1-3/4", 1-1/2", 1-1/4" have all been machined this way with beautiful results, without having to resort to two tools.

Let the CNC do its thing, move away from full forms on anything bigger than 2threads per inch.

standing by....

Fred the thread

[Mcgyver]

Originally Posted by metx I think the helix angle of the thread is whats doing it.

that would be my guess.....how many do you have to do? if not a lot I'd grind a hss bit with the right clearance angles for that helix and be done with it....somewhere on the net is a proggy where you input # starts, pitch and dia and it spits out the angles....i'd don't know enough CNC to follow Fred's described process, however if the tool doesn't have enough clearance, its going to bind and break regardless, right? you can still do all the fancy cnc tricks once you've ground the right tool for this job.

[Fred the thread]

Hi guys,
that is the point of generating the thread profile.
The suggested tooling has NINE degrees clearance down the sides and will definitely not rub.
When using this method of thread turning, although the part-program looks very long, because the tool is not engaging the workpiece with ever increasing contact lengths, standard cutting speeds can be used, and the thread is ALWAYS correct first time and every time. Number of parts per hour will be better than full forming and more consistent in quality and size. Chip control is never a problem, the inserts and holders are standard off-the-shelf products and they are versatile, not fixed to a thread form or thread pitch. Oh yes...and they are cheaper than full form inserts!
Win - win - win!
standing by....
Fred the thread

[Mcgyver]

Originally Posted by Fred the thread The suggested tooling has NINE degrees clearance down the sides and will definitely not rub.

Fred, you are absolutely right - for some inexplicable reason i was thinking a 3 start thread where you need to grind the a big clearance on the left and none on the right . I would be forming this thread profile in bits and pieces rather than a with a full width cutter to reduce cuttng forces...... if carbide is shattering, hss will get the part done.