I've got a sleeve coming up to machine, mostly pretty simple except it's made from Inconel 600 and is about 11" O.D. x 8.5 I.D. and 36" long, the customer is sending us a chunk to rough out, then we send it back for them to age harden it or something then we get it back and finish machine it. I've never cut Inconel in a CNC but I know it work hardens easy, the biggest worry is some internal grooves that are about 3/8 wide and 3/16 deep with a .06R inside corner radius and a +/- .002 dia. tolerance, these are located about 10" deep from the end of the part, is it going to be possible to rough the groove, do a semi-finish cut, check size and then take a finish cut with a standard .125 wide grooving insert? Or is it going to work harden while roughing and give problems trying to finish? The O.D. has a 3mm pitch thread too, any tips on how to thread it as far as what size cut to take and finish cut size? Any help would be great.
Follow along with the video below to see how to install our site as a web app on your home screen.
Note: This feature may not be available in some browsers.
Largest Manufacturing Technology Community on the Web
Stay Connected:
Tips on grooving and threading Inconel 600 in CNC lathe
- Thread starter Cuda
- Start date
- Replies 17
- Views 7,369
jrmach
Titanium
- Joined
- Jun 9, 2012
- Location
- Boise,Idaho USA
Good one,,April Fools is tomorrow.
That would be one heck of a project
Limy Sami
Diamond
- Joined
- Jan 7, 2007
- Location
- Norfolk, UK
April fool or not, but with a job like that, the phrase ''f*** your luck'' comes to mind.
I wish it was a joke!!! The fun part is I get to make it in steel first and they will inspect it and then and only then will they send the real chunk!!!
Limy Sami
Diamond
- Joined
- Jan 7, 2007
- Location
- Norfolk, UK
In that case - see if you can get hold of a short of the material, then at least you can play with getting that groove right by leaving the tools out of the turret far enough to reach to depth etc etc.
Find out how much a replacement piece of material is ! ........and who's liable for it
Personally I think they MIGHT looking for a patsy, anyone who does Inconel and the like has quoted a fortune, or told them to think again, so they're trying to palm it off.
Please please. BE CAREFUL!
gregormarwick
Diamond
- Joined
- Feb 7, 2007
- Location
- Aberdeen, UK
Talk to Horn about the grooving. We have a company local to us who makes a lot of large, complex turned parts (I have seen some of the drawings - tiny grooves, big grooves, angled grooves, face grooves, grooves at the bottom of holes, grooves everywhere) out of 625 and 718 who work closely with Horn. I have also had our local Horn rep in to help me with inconel. They have a good handle on it.
PixMan
Diamond
- Joined
- Jan 30, 2007
- Location
- Central MA USA
Not nearly as bad as it could be, relax.
It's Inconel 600 not 718 H1150 so tools will actually hold up pretty good, relatively speaking. The bore is huge at Ø 8.5" so a groove 10" deep allows the use of a very sturdy internal grooving bar.
It's Inconel 600 not 718 H1150 so tools will actually hold up pretty good, relatively speaking. The bore is huge at Ø 8.5" so a groove 10" deep allows the use of a very sturdy internal grooving bar.
Derek Smalls
Stainless
- Joined
- Jan 6, 2014
- Location
- Coventry RI
Just keep in mind, You NEED to keep the tool cutting! No baby feeds and never let the tool rub without taking a chip. Keep a sharp edge and as long as the tool is producing a decent chip you won't have a huge problem with work hardening. That's gonna be tough with the grooving.
I've found feeding straight in on threading works best. When you cut on only one edge of the tool the other side is dragging and will tend to work harden the back side of the thread. Keep your speeds down and feeds moderate.
I've found feeding straight in on threading works best. When you cut on only one edge of the tool the other side is dragging and will tend to work harden the back side of the thread. Keep your speeds down and feeds moderate.
Inconel comes in many flavors. Inconel 600 is not as difficult to cut as 625 or 718 but will tear more than those others....possibly a bit on thread flanks.
The following speed advice is not intended for you to run at these same speeds but should give some relative numbers comparing different types of materials. They are real numbers I use on these materials.
Threading - I use a modified flank infeed about 5° off the flank (zig-zag modified infeed with Okuma) and leave about .003" diameter to clean up on last pass with an additional spring pass. About 150 sfm with Sandvik's older 166 threader in grade 1020. For comparison, I run the same threader at 375-400 sfm in 316SS and about 100 sfm in Inconel 625.
For standard OD turning with a Sandvik VNMG 331 MF 1025... about 225 sfm in Inconel 600, 550-600 sfm in 316SS, 150-175 sfm in Inconel 625.
The following speed advice is not intended for you to run at these same speeds but should give some relative numbers comparing different types of materials. They are real numbers I use on these materials.
Threading - I use a modified flank infeed about 5° off the flank (zig-zag modified infeed with Okuma) and leave about .003" diameter to clean up on last pass with an additional spring pass. About 150 sfm with Sandvik's older 166 threader in grade 1020. For comparison, I run the same threader at 375-400 sfm in 316SS and about 100 sfm in Inconel 625.
For standard OD turning with a Sandvik VNMG 331 MF 1025... about 225 sfm in Inconel 600, 550-600 sfm in 316SS, 150-175 sfm in Inconel 625.
Philabuster
Diamond
- Joined
- Jul 12, 2006
- Location
- Tempe, AZ
FYI, this is not going to do much good if you have never machined Inconel before. Your ENTIRE PROGRAM will need to be changed around, edited, tweaked, re-worked and then some.
Inconel 600 is really soft and gummy. The stuff cannot be age hardened, so I would guess the customer just wants to do an in-process stress relieve on it before final machining.
I have never seen a shop make money on their first Inconel job before. The shit is NOT just tough stainless. Whole nother ballgame.
I will bet money the raw material the customer is providing is worth more than the CNC lathe you are using to cut it.
Here is some technical data on Inco 600 from first Google result:
INCONEL® alloy 600 (UNS N06600) Ni 76.0, Cr 15.5, Fe 8.0 Description
INCONELDAVE
Aluminum
- Joined
- Mar 29, 2014
- Location
- PA
I hope your quote was in the 15k range, EDIT no make that closer to 25k.
Good luck
Good luck
Yeah, I know the steel program will need work, but it's just to show the customer we have all the details figured out and correctly placed, thanks for the link too.
Well the lathe was about 250k in 2006 so that would be some pricey material!!!! I'd hate to scrap that chunk!!!
No clue, I'm just the poor sap that get's to machine it!!!
JLaugh
Plastic
- Joined
- Jan 21, 2015
- Location
- East Tennessee
Little .5" bars of elgiloy are about $70 dollars a foot so, The size of inconel you are talking about could hit 250K pretty quick. Cutting a sample out of steel then going to inconel is like learning to ride a moped then jumping on a super bike.
jrmach
Titanium
- Joined
- Jun 9, 2012
- Location
- Boise,Idaho USA
Cuda,don't forget the pictures,,,or it never happened.
Yeah. I'll post up a few, not even sure when this will happen, I just started roughing the steel sample when I hit a snag on the print, we have a print made in 1975 and then converted to a modern drawing last year, seems an angle and a length they want just won't work out in real life, now we got to call and find out which one is correct, this could take awhile knowing these people!!!