Carbide inserts that don’t need to be ran at crazy high speeds

[Bradsc1989]

For starters, I’m admittedly not super experienced with cnc machining so take it easy on me. over The past year or so I’ve taught myself how to program the cnc lathe at my job. As you might expect this has been a pretty monumental task but I’ve gotten the hang of it for the most part. One issue I’m running into is tooling. The machine is a fryer et18 lathe and the max spindle speed is ”only” 2000rpm. It seems like most all the inserts I’m finding, if I go off of the speeds and feeds on the packages will want spindle speeds in excess of what this machine can do along with feeds and depth of cuts that Are also likely beyond the ability of this machine. In all honesty, once above about 1500 rpm it Seems kind of sketchy. I use a lot of cnmg inserts but I know I’m burning Them up sooner than I should be by running them outside of what the package says which I assume is their efficiency range. I use mostly sandvik stuff because they have the most useable website in my opinion, but it seems like they only have the newest highest tech high speed machining in mind . The turret takes 3/4” shank holders. I guess my question is, where can I look for inserts that are happy running at lower speeds than the newest industry standard stuff. Work with a2, 4140, and cold roll a lot. Small amounts of aluminum Here and there. It’s a job shop not a production shop. If there’s anything I need to clarify just let me know

 

[john.k]

You need sharp edge positive rake inserts .....thse are commonly Chinese sold cheap mail order for alloy ,but work well on steel too with low speed/low power lathes.

 

[sfriedberg]

I found a roughing insert that does surprisingly well at low speeds and small feeds on steel. By that I mean the finish is unexpectedly much better than the half-dozen finishing inserts I tried on the same machine with the same semi-gummy 1018 steel. Iscar CNMS432-12 IC20. Fits in a CNMG toolholder. Does not leave a mirror surface, but leaves far fewer rips and tears on the surface.
That is not meant to contradict john.k. Sharp positive rake inserts also work in this situation, but the edges are much more delicate. If you think you are burning up CNMGs (which is another discussion), then expect even shorter life from CCMT inserts.
You should have a good look with a good magnifier at several of your "burned up" inserts. There are photo guides from all the major insert makers which will help you diagnose the specific kind of damage you are doing to your inserts, and suggest specific remedies. Damaging your CNMG inserts from too-low-SFM alone is going to be pretty unusual. On close examination, you may find the low lifetime of your inserts is due to something else.

 

[EmGo]

I'm wondering what we are calling "bad life" ? Because you are only supposed to be getting about fifteen minutes per corner out of a cnmg. Maybe more now but still, they are not forever inserts ...

From the description of his situation I'm gonna peddle my favorite again, the knux. I don't know why they aren't more popular. In any kind of positive rake situation they work excellent -- and you don't have to buy from sandwich.

 

[Limy Sami]

I'm wondering what we are calling "bad life" ? Because you are only supposed to be getting about fifteen minutes per corner out of a cnmg. Maybe more now but still, they are not forever inserts ...

From the description of his situation I'm gonna peddle my favorite again, the knux. I don't know why they aren't more popular. In any kind of positive rake situation they work excellent -- and you don't have to buy from sandwich.

+ 1 on the KNUX

 

[William Lynn]

I ran mostly PH 4140 using various diameters. I don't think I ever went over 800 RPM on an OD cut. I wasn't on piece work and didn't have a rate. I got done what I got done and as long as my part didn't shut down production, nobody cared. Mostly used CNMG 432 K except when needing a DNMG for a certain feature. Insert usage was not a problem at this RPM, obviously.

 

[L Vanice]

I agree that sharp positive rake inserts work as well as a ground HS cutter with similar geometry, whether you run at a slow HS RPM or way faster. I have been using TPG221 inserts in my Hardinge lathes for 40+ years, using inserts that cost $1 each or less back then and have not bought new ones in at least 25 years. I do touch up the point if it gets chipped, which makes the inserts last a lot longer. So yes, I am not up on all the latest inserts. I got a holder and some new carbide parting inserts to try in the Clausing, but have not had a job for it yet.

I saw EG's KNUX rave a while back and was quite willing to try some. But I could only find 20 mm and 25 mm holders. The Hardinge OEM tool holders only use 3/8" shank tools. I use 1/2" shank tools on my Clausing, though the Multifix holders can go up to 20 mm. Have to check whether a 20 mm holder will be able to adjust to the spindle center.

Larry

 

[Beauvais]

Seco CCMT tp2500, they have a high ideal sfm but they wear very well cutting small dia 20-30mm at 2500rpm and leave a perfect finish. Older grade but there are still some on ebay.

 

[marka12161]

Moltrecht's book on shop practice says the primary factor that wears out cutting tools is surface cutting rate. He states that this factor is more significant than depth of cut and feed rate. If i'm not mistaken, he's referring to both high speed steel tooling as well as carbide tooling. Based on this, i was always under the impression that carbide tooling allowed higher SFPM than HSS but did not require it. Am i missing something?

 

[Bradsc1989]

I found a roughing insert that does surprisingly well at low speeds and small feeds on steel. By that I mean the finish is unexpectedly much better than the half-dozen finishing inserts I tried on the same machine with the same semi-gummy 1018 steel. Iscar CNMS432-12 IC20. Fits in a CNMG toolholder. Does not leave a mirror surface, but leaves far fewer rips and tears on the surface.
That is not meant to contradict john.k. Sharp positive rake inserts also work in this situation, but the edges are much more delicate. If you think you are burning up CNMGs (which is another discussion), then expect even shorter life from CCMT inserts.
You should have a good look with a good magnifier at several of your "burned up" inserts. There are photo guides from all the major insert makers which will help you diagnose the specific kind of damage you are doing to your inserts, and suggest specific remedies. Damaging your CNMG inserts from too-low-SFM alone is going to be pretty unusual. On close examination, you may find the low lifetime of your inserts is due to something else.

This is a great idea. Thank you.

my thought process behind “burning“ them up is I’m having a hard time with chatter and gradually lose surface finish. I think a lot of the chatter is coming from not having a good starting point for speeds and feeds. I usually. Try to figure out what the manufacturer suggests on the package and scale that back to run on this machine. Sometimes it works and some times it doesnt so well. A lot of times to Get the chatter to go away I wind up feeding so hard it leaves a rough finish, not rough like it’s ripping material but just where the feed is outrunning the spindle. Almost like it’s cutting a super fine thread. If that. makes any sense? I’m probably not explaining that very well.
im probably being a little over conservative with my depth of cuts also. On 4140 about the deepest I’ve gone is 1.5mm. I’ve ran sandviks calculator before and they’re suggesting like 3mm a lot of the time. I’m not 100% on what the machine can handle. Like I said I’ve taught myself all of this. I’m kind of getting to working out the details now and I just feel like Im doing something wrong with running these inserts out of the range suggested by the manufacturer

maybe there is a calculator someone may know about that works better for lower power machines?

 

[Bradsc1989]

when I go back to work tomorrow night I’ll get a list of what all tool holders I have. I’m drawing a blank right Now and all I can think of is cnmg and maybe I use a tnmg for a finisher a lot? But I’d say 90% or what I turn is with a cnmg

 

[Beauvais]

I have some Seco VBMT160402-MF2 Grade TP3500 which If I remember say 0.3mm for the ideal doc.

How much power is the machine?

 

[Bradsc1989]

I have some Seco VBMT160402-MF2 Grade TP3500 which If I remember say 0.3mm for the ideal doc.

How much power is the machine?

10hp. 3058lb thrust on X and 3504 on Y. Weighs 2500lb. Not sure if the thrust or weight is relevant but seemed like it might be. The website also says 2500rpm on the spindle but I’m 99.99% sure ours only goes to 2k, that’s all info off the website and ours is around 10years old iirc. Also, now that you mention it, I also use vbmt for finishers. a while back i had a whoopsie and buried one like 2.5mm deep in 4140 running 1800rpm and .250mm/rev, 102mm length of cut, and it took it. thought I had a cnmg tool called up. I think it was a vbmt anyways

 

[john.k]

Yeah ,well ,I dont consider 10hp to be a low powered machine .....you should be able to run just about any negative rake insert with chip coming off red hot from 4140..............my advice was for a low powered machine of light construction ,and can be disregarded..

 

[animal12]

I don't no much past nothing about inserts or your machine , Is everything as thight as should be , gibs tight & not budging in one way or another ? I know double checking this on my old lathe helps .
animal

 

[Bradsc1989]

Yeah ,well ,I dont consider 10hp to be a low powered machine .....you should be able to run just about any negative rake insert with chip coming off red hot from 4140..............my advice was for a low powered machine of light construction ,and can be disregarded..

The spindle rpm seems to be what im fighting more than power. 2000 is all it will do but I’ve put the numbers off the packaging into calculators and a lot of them wind up well past the rpm capability of the machine. Like wellll past it

 

[Bradsc1989]

I don't no much past nothing about inserts or your machine , Is everything as thight as should be , gibs tight & not budging in one way or another ? I know double checking this on my old lathe helps .
animal

Yea we had a factory tech come in a few months ago to do a service on it and he gave it a clean bill of health

 

[john.k]

The speeds and feeds quoted are likely for enclosed machines with high pressure flood cooling..........even though inserts can run red hot ,a slight increase in temp and they burn up.

 

[Mud]

Here's an insert that will work for sure. Iscar CNMG 432 TF in 9025 grade.

ISCAR CNMG432-TF CNMG120408-TF New Carbide Inserts 5591667 Grade IC9025 6pcs | eBay

Find many great new & used options and get the best deals for ISCAR CNMG432-TF CNMG120408-TF New Carbide Inserts 5591667 Grade IC9025 6pcs at the best online prices at eBay! Free shipping for many products!

www.ebay.com

I use them in CNC and on manual lathes. I cut 4140HT, 1144 Stressproof and 1026/1018, etc. I can't remember the recommended speed and feed but a 2" dia in a manual lathe I'd turn about 500-800 rpm dry because it would be fast enough to get a nice finish without slinging a dangerous shower of chips. In a CNC with coolant probably 2000+ rpm unless I really wanted to eat up material on a long run. For heavy roughing I use the same grade with a roughing chipbreaker. The TF chipbreaker is very forgiving of feed, it will semi rough and will still break chips at a slow finishing feed. The 9025 is very long lived, If you can't make this work, it's NOT the insert
It will NOT work on aluminun though.

 

[EmGo]

So just to upset the speculation applecart I went and looked at the lathe. Can't tell much because the website sucks balls but it's an 18" lathe, enclosed, 10 horsies. At least going by the specs it's not a toy. Unless you are running 1" stuff you should have no problem with whatever inserts you want.

Sandvik guy always told me about 15 minutes per corner. Run about 400 fpm. I always like a good 3/16" or better depth of cut and at least .015" feed. WIth negative rake and softer material you have to push a little harder to get a shiny finish and yes, push harder means feed lines. You can widen up the nose radius a bit to make that less visible. Or raise the speed and use neutral rake or positive rake. When you hear the chips hitting the enclosure like a machine gun, then you're running about right. Quit treating it like a Gerber baby and make the thing take a cut.

Just try different things and see what works for you, like we all had to. There's no "secret formula" in some book that will make your troubles all go away.

I still like knux for aluminum, stainless, and other materials that like positive rake

I saw EG's KNUX rave a while back and was quite willing to try some. But I could only find 20 mm and 25 mm holders.

Now I'm flattered so had to go look They don't make those inserts in a smaller size so might be a little overkill on a smaller lathe ? But the geometry is the same, should still work good. They aren't a high-horsepower insert like a cnmg543 ...

I looked a little, smallest I could find was 20mm shank, which one could mill down but at the cost of tools and holders these days, I can understand plenty of trepidation. Going with midrange holders and inserts one could get a single holder and package of inserts shipped to US for $100. That's still kind of speculative and if someone ends up not liking them I'd feel guilty, but if anyone wants, we can do that. I think they are nice but I like Vincent Black Shadows and Ferrari Testa Rossas, too. And the occasional 67 Caddylack Eldorado

Just pour the coals to it, op. Make it take a cut. At least then you'll be removing some metal along with wearing out the edge. You're probably just rubbing it to death. More than three times is a sin, you know.