Threading Inconel

[yosimite_33]

Hi all , I got a job in the shop last week, its threading Inconel tubbing. I set the job up and started running. Im running a can cycle threading on it. I have only been able to get one thread per one edge of an incert. On this can cycle it takes 5 clean-up passes. The incert is chipping on the clean up passes. I have figured out that as long as the tool is under presure it does fine. I'm useing a 908 grade isscar incert. The rep said it should do the job. I'm also useing a 1" bar, thanking about ordering a carbide threading bar, the boss is going to scream when he see the pirce of that bar. I don't know what else to do to keep the incert from sucking in to the inconel on the dry passes. I just got some info one 2 line programing, but I haven't had a chance to try it yet. Has anyone had this problem befor ? Thanks for your help.

[Chrliev]

Inconel is a soft but tough metal to machine, it tends to weld onto the edge of carbide inserts and end mills and then when the build up flakes off, it takes a little bit of the edge of the insert off with it, the insert appears to become dull very quickly but its actually broken or chipped and then generates a lot of heat making things even worse.

You don't say what type of machine or CNC control. Try coming into the thread on a 30 degree infeed instead of straight in. That is every pass should come down one side of the thread not straight down the middle, this makes more of a ribbon chip and eases the tool tip pressure. Fanuc controllers are able to do this in the G76 canned cycle (A code?).

The other thing is you should be using a C2 (cast iron) grade of carbide, it should be the softest and most shock resistant carbide that you can find, coatings help, cobalt M42 hss actually works better than carbide but they don't make threading inserts in hss. Use plenty of cutting oil instead of a water soluble coolant to increase lubricity and reduce chip welding.

That's all I've got, I hope it helps you...

Charlie

[yosimite_33]

we have the pumma 300 and 300m. They use the fanuc control . I will try the G76. Would you know what format you need to go with the G76 ? Like G76 X0.0 Z0.0 P? Q? R? and what else gose with it ? I'm new to the programming world. I'm cutting a 1 3/8 -10 stub acme id thread. I will look into the softer grade of incert. The rep did say something about a 205 grade, I have read some where that this inconel cuts like copper, so using a softer incert makes sences. Thanks .

[Chrliev]

Yes, for an ID thread it goes something like this:

% (PROGRAM START FLAG)
:1076
N5 G90 G20
N10 T0606 M08
N15 M03
N20 G00 X1.2
N25 Z0.1
N30 G01 Z0.01 F0.012
N35 G76 X1.375 Z-3.5 D312 K0.125 A60 F0.1
N40 G00 X4. Z0.1
N45 Z3 M09
N50 T0600 M05
N55 M30

X = Major Diameter, Z = Depth, D = Depth of first pass, A = Angle, F or E = Thread Pitch.

Assuming a thread depth of 1/8"? Position slightly away from the face at a clearance dia smaller than the hole. I think your acme thread probably has a 29 degree angle so A would be 29.

Important Note: Please try this on a test part first, as I make no claims for accuracy, in a previous life, I used to do this all day every day, but I haven't cut a thread on a CNC lathe in over 20 years...

[PixMan]

You don't say just which model Fanuc control that is. MOST use a two-line G76 cycle, others use the one-line G76 shown in Chrliev's post.

The two-line version of the program looks something like this:

G0 X1.2 Z.1
G76 P010029 Q10 R5
G76 X1.395 Z-3.5 P400 Q50 F.1

In the first G76 line, the "P01" is the number of "spring passes" at final depth, the "P0100" is the amount of pullout as a unit of thread pitch (I always use 00 unless the requirement is for slow pullout for strength), and the last pair of digits in "P010029" is the compound infeed angle to be used. The "Q" value is the smallest increment of infeed to be used before the finish pass allowance (a.k.a. clamp value, it won't take any less than this, per side). The "R" in the first G76 line is that amount left for the final pass. After it makes that last pass (in this example, .0005" on a side or .001" on diameter), then of course the first pair of digits in that first P kick-in for number of spring passes.

Now the second G76 line:

"X" (1.395 in this case) is the final diameter value. The cycle retracts to the X1.2 starting point before backing up the Z axis for the next pass. the "Z" value is the endpoint of the threading cycle in Z, most often a negative value on chucker lathes like your Puma. The second "P" (400 in this case is .040") is the height of the thread. In this case, it is a "per side" (incremental) height, subtracted from the X1.395. The cycle never actually makes any cut at this (1.315") dimension, but uses it for calculating the first pass. The "Q" in the second G76 line is the depth of the first pass. Here, the "Q50" is .005" per side, or .010" on diameter. So... the first pass will actually be taken at 1.325". The "F" is your lead amount, or "feed per revolution".

In feeding in, this example uses a 29º compound infeed. The first pass will be at 1.325", the last pass before the (.001" on diameter) finish pass allowance will be at 1.394", and be .001" deep per side. The control will automatically make depth-of-cut adjustments downward from the first .005" depth-of-cut at 1.325" all the way to 1.394", but will stop going down when it reaches a .001" clamp value. If the cycle takes too many passes, you can reduce the number by using a higher "first pass depth" and smaller "clamp value" amount. Because Inconel just loves to work-harden if you don't "stay in the cut", I'd probably try using a "0" in the first-line "R" and a .0075 as the 2nd-line "Q". Note that some controls will alarm out if you use decimal points in the P, Q, or R, some controls are OK with it. Either way, if you just skip them and remember to have 4 places to the right of where a decimal point would be (for machines running INCH mode only!) you'll be OK. Deleting leading zeroes is OK, deleting trailing zeroes is NOT OK.

In the case of Inconel, there are about a dozen different alloys and many different tempers for that type of high-nickel/high-cobalt material. Which alloy and what temper is your material? Most Inconel tubing will be Inconel 625. Try a Vardex 3IR10STACME grade VTX or a Walter NTS-IR-16 10STACME grade WXM20. You'll get much better results than that Iscrap insert.

BTW, the reason I have the major diameter of the thread at 1.395 is because that's what it is for a 1-3/8" stub acme thread according to data I found. I recommend you go to Vardex's website and download their "TT GEN software for threading. It's GREAT!

[yosimite_33]

Chrliev, that is the can cycle that they have been trying to use at the other plant, an that is what we started using. But it just has to many dry passes. I'm going to try the 2 line program so I can set it up for no dry passes or spring passes. I do thank you for all of your information. You have been very helpful.

[yosimite_33]

Pixman, All that info is great ! thanks , I thank this will help with our problems on this inconel. I have sent a insert request to vardex and walter so they can put me in to contact with the reps. our pumas have different version of the fanuc control. some have 18I, 21I, 32I . We had it set up on the puma 280 it has a 21I we pulled it off of the machine and tryed to run it on a 300 but the new soft jaws will not get small enogh to hold the matteral. we are trying to find some longer soft jaws.

[PixMan]

To reduce to perhaps eliminate the spring/free/dry passes (whatever you want to call the passes with no infeed), run the program similar to this:

G0 X1.2 Z.1
G76 P000029 Q5 R0
G76 X1.395 Z-3.5 P400 Q75 F.1

This will make the machine run the cycle with .0075" depth-of-cut (per side, or .015" on diameter) for the first pass, and .001" on diameter as the last. It may still take too many passes. If so, increase the 2nd line "Q" value to take a bigger first cut. The differential between first pass depth and "clamp value" (the 1st "Q") is what determines how many total passes it'll take, and the progression.

What you will probably find is that no matter what you do, it will still take ONE free pass at final depth. This is something built into the cycle by parameter settings of something internal of most (not all) machines and I've never been able to solve it. Still, one is better than 3.

[yosimite_33]

ok thanks, I will give it a shot and let you know what happens. Thanks all that helped out .