O/T coated cutters

[Lars Christensen]

As you know, I am new to this milling, so there for please bear with me.

 

I got into a lillte discusion with a guy today about coated tooling(endmills).

He told me that coated carbide cutters would not exnend tool life in soft steels like D-2, A-2, 4140, verses standard carbide. Now with my limmited experince, it seems to me that it does. But if its worth the cost, I am not sure.

I would love to get some feedback from you guys on that.

 

Thanks

Lars

[Rekd™]

It depends on the coating.. if it's the wax coating they put on EM's after regrinding, or the felt marker coating, then no, it won't increase tool life.

 

Any other coating will.

 

'Rekd

[Keith Graydon]

O 'rekd. you're so subtle.......

 

Lars, What was your "friends" argument why it didn't matter? just curious. I like coated nserts and cutters too.

[Toolfab]

I mill A2 everyday...all inserts are coated, but our endmills are not. We have flood coolant on our machines and really haven't ever had an issue with uncoated endmills.

 

[cadcam]

I like the wax tools ,that way I can burn them at both ends.

 

On reked statment +1

[Jean-Simon]

We were using OSG ball mills for finishing 3D shapes with TIALN coating and man you never see the end but as others mentionned before when they were coming back from regrind (because we had some flats that needed regrind) it was like if they'd paint it. I saw some cheaps endmills (carbide with supposed TIALN) coating that wasn't changing nothing to life because they didn't have any anyway! All that was also in D2-A2 P-20.HTH!

 

 

Simon

[godzillia_dude]

+1 Rekd (I liked the wax or felt marker comment )We use alot of TIALN coated and get great tool life on various materials. Lars, ask the gentleman that you were discussing this with if he also felt as though Nitrous Oxide didn't do much for the temporary performance of cars

[fboike]

Lars,

I had some cheap 1/4-20 taps TIALN coated.

As a referance they out lasted blue diamond.

15 to 1. in cpm 15V. so I would say coating

does improve tool life.

[Müřlıń®]

I get double and even triple life out of TIALN coated inserts. But only if its on the right kind of carbide.

 

I think it depends on the rigidity of your machine. For my older machine, I must use carbide that is somewhere in the middle as far as density goes or the edge gets fractured too easily.

 

I have no use for the gold coating. I have seen plain carbide that is of good grade out last inserts that have been coated with that stuff.

 

 

Murlin teh my .02

[Ron Branch @ 5th Axis]

Well I wil throw this example out there and you make what you will out of it. I was doing 440 ss casting with 1" deep by 10" dia worth of material out of 4 faces on a square casting for a agaitator hug. I was going through about (10) 1/2" Carbide endmills flooding it with collant. I use to do anywhere from 4 to 10 casting at a time. My tool bill alone per part for them was $325 a part. I hated it I tried everyone's uncaoted endmill and coated Tin endmill about the same results. I then got the fullerton TIALN 3/4 3 Flute Carbide endmill. I then used only a mister with no coolant just for air to keep chips off the part. I paid $85.00 for the tool and was able to do 4 hubs with one and cut 3 hours each off the job. Same results when cutting s-7 and a-2 tool steel for die blades. Run Tialn dry the coolant creates thermal shock that is to much and causes stress fractures which fatiuge the tools.

 

Just my 2 cents

 

Crazy Millman

 

[ 09-17-2003, 10:39 PM: Message edited by: Crazy Millman ]

[Harryman]

Ever get any similar results with 304 SST? I'm ruuning wet and slow. Every time I try to crank things up to what the tool salesman says will work... BOOM.

[Ron Branch @ 5th Axis]

Harryman are you using high helix or slow helix for doing it. I also find that if dont give yourself good chip evacuation it causes alot of problems when cutting 304. I would maybe decrease my depth of cut and then increase my feed load per tooth. I like to have it at like .005 to as high as .009 per tooth. I would problay look at how you are holding your part keeping any vibration out of them also how much you have sticking out of the holder if you are cutting .5 deep I would get a stub endmill and have .6 sticking out. I am sure you have thought of all of that just throwing it our there. I use to run as high as 150 sfm of Tialn endmills. If you are looking at inserted tools I had good result with inserts that had postive rake and no coolant. If using facemills I like the Mil-Tec line here is the link:Mil-Tec Cutters

 

Good Luck I hope that helps.

 

One other thing if using uncoated and coolant then I would kick my mixture up to like 20% to 30% for good lubircation. If you have not cleaned out your tank in a while get some baking soda 1 cup to one gallon and use it to clean it out to kill most of the bacteria. If you coolant has not been changed in more than 6 months it can effect your cutting.

[Lars Christensen]

Thanks guys, just the answer I was looking for

I will keep on runing my coated endmills, and when the guy is looking over at me I will give him one off these .

His reason was basiclly that"coated endmills onely is a penefit in hardend steel".

I am runing a Haas Minimill with onely 6000 rpm, as max. My way to tackel jobs have been to rough pockets and other applications with (forexamble-a 1/2 Tialn Garr cutters)

200% feed and 150% speed, and then onely taken 0.015 steps, with the theory that I am protecting the machine for accuracy(man, had to look that word up in my danish dictionary(had to look up "dictionary" too )with onely having 6-10% spindel load. I have to try to run without coolant tommorow.

If you guys would comment on that tecnic too, then I do not know how to thanks you enough.

 

Thanks again

 

Lars

[MACHINEMASTERG]

harryman we cut alot of 304 and 316 ss first we buy the l series and the good mix its controlled better i belive in the nickel content then we do light deeps of cut with fast feed rates and tialn coated mills dry with an air blast the tip will wear but we go thru the part into the fixture 2x the depth of cut works great and no shattered tools

[Keith Graydon]

quote:

---

the tip will wear but we go thru the part

into the fixture 2x the depth of cut works great

---

+1

 

the corners of the cutter takes the most abuse.imho

[Müřlıń®]

quote:

---

Run Tialn dry

---

+1

 

Murlin

[Lars Christensen]

Ok ,just came home from the shop.

 

Tryed to mill a slot (4" long, 1.74" wide, and 0.5" deep) with a Garr 5 flute coated endmill.

in D-2,

I started out with 3455 RPM and 103. Feed/min. 0.01 step, and without coolant, took about 10 min before there was sparks flying and the steel turned into, Hmm ocean blue water coulor, So I changest cutter, and dropped the feed down to 84. p/min, but still the cutter and steel turned worm, so I threw some coolant on there, just so I could finish up this first part.

Now my biggest problem is that I still have 15 of these slots to do, and Im runing low on cutters. And since my good friend is in "rank" higher than me, I know that I will hear bull****, if I want to ordre more coated cutters.........please help..............would like to have written this with Caps on, because I verly feel like screaming.but is trying to stay come, with the hope that one of you guy's will help me.

 

Thanks

Lars

[F. JAVIER]

It seems to me that you are running a little high on your sfm and about twice as heavy on the chipload. Mabye you are using HSM method for roughing or mabye I don't understand what you mean when you mention "step"; I last cut D2 at 280 SFM and .0025 chipload on a .5 CEM (uncoated) translating to S2140 and F26.75. my step was about .1" deep.

My experience with coated inserts has been good (cuting dry) but this was in SS.

Good luck

F. Javier

[Müřlıń®]

quote:

---

I started out with 3455 RPM

---

****Gulp*****

 

I'm surprized it lasted 10 min.

I'm not that big on HSM strategy though.

 

 

Murlin

 

[ 09-19-2003, 08:49 AM: Message edited by: Murlin ]

[Toolfab]

When milling A-2, FYI, I use S916 and F2. (ipm) flood it with coolant, and un-coated end mills. That is what I use, it has never blazed up a tool (unless I forget the G1... )

 

HTH

 

 

(should note that I use 4 flute em's)

 

[ 09-19-2003, 09:22 AM: Message edited by: Toolfab ]

[fboike]

Lars

I would run a 1/2-5 flute, 300 sfm, .008 fpt

.05 doc, thats 2300rpm, 92ipm. depending on

horsepower you may need to take less doc.

the key is to get the chips out of the slot.

if you start recuting chips the cutter is gone.

hope this helps I hate people standing over my shoulder.

[Hardmill]

Sounds to me like your cutter has too much

relief. Do you have a link for supplier,

P/N etc.. I'll take a look at it for you.

 

PEACE

[Lars Christensen]

Thanks for all the replys.

I allmost got the job finished up last night, with your guys help!!!!

 

F.Javier, step should have been "doc", just couldent come up with the word.

 

Hardmill, it is a 1/2 Garr cutter, think it has a 255m number on it, do not have a link.

 

Long story:

I have been a pure EDM guy the last 8 years, the last time I had a Endmill in my hand, was back in Denmark when I took my aprentienceship as a moldmaker, and then it was on a bridgeport using HSS endmills, where we looked at the endmill spinding, and then desided that that looked pretty good for speed. Now I am trying to run this MiniMill next to my wire. Now I realize that I got to do some homework, I am getting a handel on programming in Mcam Mill, and I think I know how I want to run my jobs, BUT tooling, well here I have all the questions, why that cutter? speed/feeds? doc? chip load? other options?.

I think that I have to hook up with different tolling companys TECH. deparments, and see if they can explain to me what I need, and why.

 

Any of you guys have a good advise, how I can move from the EDM world (power settings, spark gab) into the sience off "real" tooling?.

Thinking of websites and book, or what else is there is.

Basiclly getting 10 years experince as fast as possible.

The shop I work at have mill guy's, but dont seems like that they verly know how and why. They use what ever endmill that get ordred, and use the cutting data from the manufactor. I know that it will bring you close, but my nature is that I need to understand why and how.

 

Thanks guys, you have alredy been to so much help, if any is stopping by Rochester NY, send me a mail, and there will be a cool one, with your name on it in the fritz.

 

Lars

[Harryman]

quote:

---

The shop I work at have mill guy's, but dont seems like that they verly know how and why.

---

Way too many so-called CNC machinists have no true ability to calculate speeds and feeds. If you learn how to make the calculations and pay attention to the results, you are ahead of the pack. Interpret tool wear as a resultant of two separate factors, Speed and Feed. (There are quite a few others such as recutting chips and volume of metal removed, but I don't want to write a book here.) Generally breakage, is a feed issue and burning is a speed issue. So if a cutter is burning, reduce speed but not feed per tooth, MAKE THE CALCULATIONS, then note results. You have to put some number into the machine, so make it a precise number (S486 F1.34) or what ever the calculations show. Base the calculations on surface speed and chipload per tooth for your particular workpiece/cutter material combination.

 

Calculating (as opposed to guessing) speeds and feeds is especially important when working with small cutters.

[Chris Rizzo]

Lars,

 

Recently moved to Rochester? I lived there for quite a few years while attending RIT. Nice town!

 

As far as getting up to speed on the mill, I've got two recommendations:

 

1) Get in touch with a good tooling supplier there. Make them come to your shop, look at what your doing, and make recommendations. Some of these guys are sleazy salesmen, others really know there stuff. Find a good one, and he can be a great help and save your a$$.

 

2) Take a class or two. I hav'nt been in Roc. for a while, and I'm not sure what educational programs are still running (Monroe Community,R.I.T.) Go out to the RIT campus and check out the shops there. I heard they cut the shop programs way back, but the fellas out there are great guys.