threading problem

[girishnadkarni]

hello ppl

we are into machining of duplex and super duplex stainless steel machining on turning centers and have threading operation on major components
im finding lot of problem to keep up the life of threading insert with less cycle time
threading spec 8un class 2a thread
dia 53.75 mm for a length of 40mm
75mm do
79mm do
im not able to go above a depth of cut of 0.1mm diametrically
controller fanuc oitc
can any body suggest me a good solution for this

[g-codeguy]

You may not have given us enough information to be of much help. What RPM are you running? What insert are you using? Can you give us the threading cycle you are using? I don't mean G76 2-block call either. What values are in the cycle?

Right off the top I'd like to know why you can't take more than .1mm diametrically? Never heard of such a thing. That amount is ok for the last pass, but is way too shallow for the first pass. No wonder you can't get any tool life. I wouldn't expect any unless you were cutting warm butter.

[girishnadkarni]

rpm of 380
G21 threading cycle
carmex insert 16er 8un
sandvik R166.OG-16UNO-080-4125
if at all i increse the depth of cut the insert blows off
i tried it with g76 cycle but the flank wears out quickly
and the is no provision for alternate flank infeed method in this control
any soln for this

[g-codeguy]

Looks like the 4125 should be running around 350 sfm. I assume you are using the MXC Carmex grade. That should run at least that fast also. That means you should be running around S635.

I am not familar with G21 threading cycle, so I can't help you there unless you want to post a threading cycle, and explain what each word represents so I can figure it out. Well...I think I could figure out what the X, Z, & F (or E) stand for. I've been fighting threads for a long time.

Can I assume you are running a 2-1/8 8UN thread? What does the 75mm do and 79mm do refer to in your first post? Size of the local cow pucky? Sorry, little sick humor.

Can you control compound infeed? Which G76 thread cycle does your control use? I am very familiar with those. Care to post what you have tried with the G76 cycle?

One thing to remember is that some grades of inserts won't run very well if you go too far below their suggested range. You are running around 210 sfm for the first cuts. SFM too low, and the material sticks to the insert. Next cut can cause a chunk of the insert to chip off. Also the material is probably workhardening at those DOCs.

[extanker59]

The other guys know much more about the threading cycles so I'll just ask a tool set up question: Are you sure you have the right shim for your laydown tool at that diameter? At that size, it's probably not the one that was originally supplied.

[girishnadkarni]

the material which im machining is CD3MWCuN DUPLEX STAINLESS STEEL
which contains ni, Cr, molybdenum which makes the material sticky and hard for machining
i have tried using g76 flank infeed method which does not work
nw we use G21 X53.75 Z-40 R0 F3.175
X53.65
X53.55
X53.45
.... AND SO ON TILL THE THE THREAD DEPTH IS ACHIEVED
X IS THE DIA FOR THREAD PASS
Z IS THE LENGTH
R IS USED FOR TAPER THREADING
F IS THE PITCH OF THREAD
THREADING SPEC 2 1/8" 8UN
2 5/8" 8UN
3 1/8" 8UN
THE SHIM IM USING IS AS PER THE HELIX ANGLE
NW TEL ME IS THR ANY WAY OUT

[g-codeguy]

Being in the USA I am not familar with that material, but have machined materials of similar makeup. Your G21 is like my G92. It doesn't use compound infeed. A zero degree infeed creates a tough chip. I haven't used this cycle since Hector was a pup.

Does your starting point clear the diameter so that the threading tool won't drag on the material on the return move? I ask because you said the insert keeps breaking.

Try

G97S600M3
T0101
G0X55.Z13.M8
G76P000129Q008R.076
G76X50.11Z-40.P364Q045F3.175

OR

G76X50.11Z-40.K3.64D450F3.175A50.

depending on control.

I don't program in metric, so please make allowances if I am off on some figures. I think you should be taking a minimum of .015 thousandths per side on the first pass. I tried to set it up to take a minimum cut of .003 thousandths per side and the same depth for the last pass. This is to keep the material from work hardening.

I normally use 29 or 55 deg. for my compound infeed with the 2-block G76 and 50 deg. with the 1-block G76 call. I use 60 deg. if slowing RPM doesn't eliminate chatter. It has the least amount of tool pressure.

If the insert gives problems on the first pass, lie to the control by making the P or K larger. This will give you a lighter cut on the first pass without increasing the number of cuts significantly. If you lower the Q450 or D450 by a couple thousandths, it will result in a lot more passes.

EDIT: This should be a good starting point, but realize that you may have to modify a bit. Might be able to run another 50-100 RPM faster. May need to take a lighter finishing pass. Could be you need to make a couple spring passes to hold pitch (hard on insert, and doubtful with this coarse thread). May need to try different compound infeeds. May have to give it a greater thread height, etc.