cutting inconel 718

[stsrvanvliet]

Im cutting inconel(718) for the first time and im having trouble getting my cutters to last. Im cutting grooves with a 4-flute .250 ball endmill ramping down .031 per 360deg rotion of the 4th axis at a total depth of .31. My speeds and feeds are 1075rpm 7imp at 70fpm. Wondering if those are good numbers or if im screwing myself on this? Any help or suggestions will be greately appreciated

[jmcd]

Inconel is a reel drag to cut and it wears out tools fast so make shure that you take a min. cut of .05 at all times. Try turning down your spindal to about 800 - 1000 rpm (roughly .0015 chip load per flute) use a 4 flute solid carbide e-mill or a 4 flute ticken coated e-mill and run about 10 ipm.
GOOD LUCK!!!!

[stsrvanvliet]

ill give it a shot. thank you.

[jmcd]

how did that work out for you

[stsrvanvliet]

couldn't get it to work. the cutter kept braking down to soon. the cutters did last a little longer with the adjustments you suggested though.

[ajl6549]

I don't know what brand/grade of carbide you are using but I'd try using an Iscar EBSI-A3 250-313-C250 solid carbide, PVD coated ball end mill. This is a sub-micron grade of carbide it's tough and has a sharp cutting angle ideal for Ni based mat'l. This should run at 70 sfm and about .001 - .0024 ipt or 1069 rpm and 1.6 ipm depth of cut should not be more than .0625". If you are using your fourth axis as your feed axis be sure that it's feed equals no more than the .0024 ipt above. Also be sure your tool has near zero run out in the holder/spindle of your machine tool. These end mills ar'nt cheep but they work.

[bennett71]

I have machined a lot of 718, 625, 690 & alloy 286 & none of them are any fun except for the fact that if you get to keep the chips, the scrap value is good. One thing I found that seemed to help is to mix the coolant thick for more lubrication. This will cause less cooling also, so beware of work hardening. The best advise I was ever given on this subject was from an oldtimer that sells me inserts from Ingersoll. He said if you want to machine "super" alloys, you better quote it for "super" dollars. If you give these jobs away in a quote you WILL get killed in tooling costs by the time you finish the job. Super alloys like to eat tooling & if you look @ what they are used for you can see why. Good luck!

[pepo]

Been in the machining end of the gas turbine industry for 30 years. Lots of inconel,waspalloy,stellite,all high nickel content. Its the nickel that makes this stuff tough. The secret to cutting this stuff well is realizing that it isnt hard,it is tough. There is a real big difference. You cant plow it around with dull tools like you can aluminum or steel. If steel was a choclate cake then inconel would be a loaf of hard italian bread. You can cut cake all day with a dull knife,but,try the same knife on the bread and you will saw like crazy and get nowhere. You gotta cut this stuff clean and sharp or it will work harden.

[drummond1]

I've cut a lot of inconel. Try switching over from HSS to carbide on the cutter side and reduce your sfm. Make sure you have a good cutting lubricant as the gummy nature of this material lends micrograins to stick to the tool and retain heat. Drum

[wewon]

Funny that this came up. We are running some test were I work on developing the cut-data for several materials, inconel being one of them. I will see if I can find some information to share with you on our findings.

[cdlenterprises]

Surface footage is too high. I'd run between 35 and 45. 1/4" em should put you around 640 rpm. You definitely need a coating - TiCN or TiAlN. Sometimes carbide isn't the answer in tough materials. While it is harder and certainly more wear resistant, it's much more brittle and won't give you as sharp of an edge that HSS can give. If all else fails, try a good cobalt grader em with one of the above coatings. You may be pleasantly suprised...

[wewon]

Sorry for the delay......

For Inconel 718
Tool: Uncoated carbide
Diameter: 3/4"
Rake: 6deg rake 30 deg helix
Teeth: 4
Speed: 331 RPM
Feed: 3.97 IMP
Axial DOC: .15
Radial DOC: .1875


This is just in from our lab today. Part of a larger tool life study.