Coolant and carbide...

[Tom Szelag]

So today was very exciting. I ordered my first set of cutting tools! Figured it would be nice to have my own rather than use the kinda crappy ones that have been sitting around the cabinets at work for years (we took over a student shop...eeek). And it beats having to constantly borrow good ones from the machinists I know.

 

Cut a lot of wrought aluminum alloy, some 4130 steel, some stainless steel, some engineering plastics. Do some manual work, and some CNC. So I went with .125, .250, and .375 flat EMs, 3 flute, centercut, solid carbide TiCN coated. And a .500 flat cc EM, M42 bright finish (though I regret not having gone with TiCN on that too, oh well).

 

ANYWAY. Saw in another thread some issues about thermal shock on C-2 and resultant shortening of tool life. For manual and 2-axis CNC work I only get up to about 2000rpm and 10ipm, and dab a bunch of A9 or Boellube on my workpiece. The 3-axis stuff I do only gets up to 5000 rpm and maybe 25ipm. So its not like I'm doing HSM and ripping through material.

 

So at those relatively low speeds and feeds is it fine just to flood the hell out of my work, as I typically do?

[ChuckM]

Where to start?

 

The answer to your question is... "it depends". Depends on the workpiece material, the type of tool and the PVD coating used on the tool.

 

For your aluminum milling, you will want to flood and stay with coatings other than TiAlN. On some softer/gummier stainless steels, you will also want flood coolant. Same goes for titanium and nickel based alloys.

On some of the harder grades of stainless however (or hardened stainless), you should run dry (with air blast) and using a carbon-nitride or aluminum-nitride coating. Any TiAlN coated tool should be run without coolant, as the coating needs the heat to provide that useful layer of aluminum oxide. On materials 40 HRC or better, TiAlN is the only way to fly IMO.

 

On ballnose cutters, especially end mills, you will want coolant if surface finish is paramount.

 

So it depends but you TiCN coating is much more forgiving than TiAlN. I'd still stick to dry machining unless you notice BUE on your cutting tools.

 

-Chuck

[Tom Szelag]

And what kind of speed increase can you run with a coated carbide tool?

[betts]

I wouldn't assume you can increase SFM or feedrate because you are using a coated end mill.

 

The purpose of the coating is to increase tool life and in some cases lubricity. You may gain a little if the tool is holding up better to heat when its coated, but that goes back to "depends".

[ChuckM]

General guidelines are...

 

TiN = +20%

TiCN = 40%

TiAlN = 50%

 

Then there's the multi-layer tools which can go even faster.

 

Best thing you could do is follow the tool manufacturer's recommendations, starting at the low end parameters and experimenting. Common sense also goes a long way in analyzing your setup... setup rigidity, tool rigidity, tool length, etc., and compensating for the many variables.

 

May have come across the wrong way in my last response..... your TiCN coating is by far the most applicable across different materials. For your stainless, use it with flood coolants. For aluminum, use flood. Basically, anything you cut with TiCN coated carbides... use coolant. Although I have had good results running it on mild steels with air blast.

 

Anything you decide to cut with TiAlN coating, run dry unless cutting titanium or nickel alloys. Then I'd still use TiAlN with coolant.

 

Look at the premium carebide tool makers online. I tend to like to use the ones who offer the most information on their product. However, OSG-Sossner is a very good tool maker with a pretty pitiful website... their catalog is great though.

 

-Chuck

[betts]

I may also have come across wrong in my response, but I don't buy anything uncoated so the key is where are you starting? If you are trying to use generic S&F info and ad to it for a coated end mill I don't think you will get the best results.

 

However starting with the mfrs. recommendations is the place to start, as Chuck said.

 

Again there is always a trade off. I use some awesome tools from OSG, but they are always job and task specific. Not because they wouldn't work for other things, but they are quite expensive and you can't afford to "under-use" them.

 

There are many excellent tools available and that really makes the decision making more difficult. Everyone has a cost/benefit ratio to work within so sometimes there is no way around trial and error when you aren't machining in a production atmosphere.

 

Of course usually without much arm twisting you can get a sales rep to float you tools to try on the premise that you'll buy from them if the tools work as expected.

[Tom Szelag]

"Best thing you could do is follow the tool manufacturer's recommendations, starting at the low end parameters and experimenting."

 

I'd love to follow the tool manufacturer's reccomendations, but where the blazes do I find this sort of literature? Will they come with my tools? I can't even find Accupro's website. Looked at Metal Removal, couldn't find reccomended speed and chipload data. Same with Sandvik. Maybe I'm just blind...

[ChuckM]

I found quite a bit with a quick search through various different brands.

 

Metal Removal's Maestro line is the only thing I could find of the MR lineup... didn't know they were a Kennametal company either.

 

http://www.kennametalipg.com/pdf/MR04013B-Maestro.pdf

 

I have no experience with MR, but for their general line of end mills I'd use the calculator at Robbjack's website.

 

http://www.robbjack.com/html/tech.html

 

Then of course there's Kennametal...

 

http://www.kennametal.com/images/pdf/a01-152_end_mills.pdf

 

Here's information from SGS...

 

http://www.sgstool.com/product/pdfs/HighPe...talog042004.pdf

http://www.sgstool.com/product/pdfs/Fracti...alog052004r.pdf

 

Mitsubishi Carbide...

 

http://www.mitsubishicarbide.com/mmus/en/p...diamondstar.pdf

 

Garr...

 

http://www.garrtool.com/pdf/vrx_flyer04_2.pdf

http://www.garrtool.com/customersupport.htm

 

By the way, Garr's VRX line is pretty darn good for the money. I ordered a few 1/2" 4F a month or so ago to get me through some nasty A36 job and they performed very well. Think I paid ~$37 a piece.

 

Which goes right along with what betts is saying. It's always a balancing act with tooling. I had a job recently where I really would have loved to have had a long-edge inserted cutter for a 4x dia. deep slot ~3.75" long. Problem was... we were only making 2 of these parts and I just couldn't justify the cost. A cobalt 1.25" 4F wasn't exactly cheap but it wasn't anywhere near the cost of the inserted mill either. So I roughed it to ~3-1/4" deep and left the rest for the long one. Not only that but, I can't think of a too many situations where we've really needed a cutter like that in our shop. 50 parts and I would have placed the order... but those are the situations you're faced with in a job shop.

 

 

I'd also suggest going to OSG's website and ordering their high-performance and standard end mill catalogs. Very well put together and much more informative than their website.

 

Hey, I'm tickled pink that you're an engineering student wanting to learn more about machining. I wish we had guys like you at my shop cause it'd make things a lot easier on me.

 

Take care.

[BernieT]

"I'd love to follow the tool manufacturer's reccomendations, but where the blazes do I find this sort of literature?"

 

Ask for catalogs from the mfg. Hanita, OSG, Garr. etc.

 

Also, on Jay's (CadCam) FTP site is at least one speed/calculator "MEconsultant". Also 'Milling cutter speeds'

[Tom Szelag]

Thanks folks.

 

Yea Tau, I've been using ME Consultant. Pretty damn nifty! But there's only an option for a generic "carbide" material, not uncoated vs TiN vs TiCN vs TiAlN, etc.

[Müřlıń®]

quote:

---

nickel based alloys

---

I use TiAIn coated with air.

 

The big deal with edge fracture on c2 and other cheaper grades of carbide is the condition of the edge during cutting.

 

On alu, the edge wont get very hot so you can flood. Plus, alu needs flooding reguardless due to gummy properties.

 

On steel, the edge of your carbide glows red under a cut.

 

When you flood, the edge gets quenched and becomes brittle and develops heat checks.

 

The better carbides will hold up longer during flooding, but wont hold up as long as air on nickle base alloys.

 

With air, sometimes you can use the cheap carbide and save money TNMA inserts have 6 points and cose 4 bucks. Mose of the helix inserts we cut with today only have 2 points and cost 10 bucks.

 

When it comes to mass metal removal, TNMA kicks a$$ when it comes to cost.

 

IMO

[35K chipper]

ME @ CU Boulder,

For aluminum try www.destinytool.com they make a line of tools i think are the best i've ever used for 7075 6061 2024 or mic6 alum. they call them vipers and diamond backs. example .500 3flt 1.25loc 30000rpm 400ipm 1.0doc .05radial. these tools have a coating the manufacture calls stealth. friction coefficent .023 thickness .5-1 microns. great stuff. the diamond back rougher same rpm doc and radial except 800ipm. i have to run the chip conveyor wide open just keep up.

[Chris Rizzo]

Tom,

 

With your equiptment limitations, your going to be off the low end of most modern tool manufactures chart's in most cases in regards to either rpm's or feed ability (chip load). Of course you can adjust the forumla's accordingly, but in the end your going to get your "best" feeds and speeds by eye, ear, nose, and feet (vibration)...and of course tool life. Use the "recommended" #'s to reassure yourself that your in the ball park, (especially in SFM in the harder materials), but don't be afraid to come up with what works best for your equiptment and budget.

 

hth.

 

35k chipper, I'm envious. Sounds like you need a 10000rpm conveyer

[Tom Szelag]

quote:

---

example .500 3flt 1.25loc 30000rpm 400ipm 1.0doc .05radial.

---

 

No freakin way!

[routerman7030]

Give Data Flute a try, they make really good cutting tools and are very good at helping you out. www.dataflute.com

[35K chipper]

Dataflute use to be my #1 endmill but it slipped into second place. time is money not the cost of the tool.

[routerman7030]

For most runs i did i used a lot of Dataflute stuff, but i did like the roughing endmills that Robb Jack made, they were really good in hard steel, I used to do a lot of testing for data flute, especially in aliuminum, they do make a good tool for that.

[McRae]

Tom -

 

For what you are doing - Don't Worry about it. The edge frittering and thermal shock effects will only matter on the nth workpiece. This is more a technique for High Production metal removal where the edge temperature is quite substantial.

 

Milling what you do, flood your work and keep it cool. That will help you more.

[ChuckM]

~22" long slot, .400 inches deep and .600 wide.

 

We had a similar cut in a prototype 4340 tool body. Just one part but I am willing to bet with any duration of cut like this, using a 1/2" end mill as in this case, will show signs of thermal shock using coolant. Especially considering all the intersecting slots in this particular part.

 

In anything with short duration cuts, I'd run dry. Anything where the tool is exiting cuts frequently, I'd run dry. So evaluate the work (prototype or production doesn't really matter) and then make a decision to run dry or not.

 

35k Chipper, thanks for the heads up on Destiny Tool. I'll have to give them a try.

 

Speaking of aluminum, have any of you guys used the new Weldon 3-flute ski-carb end mills? Weldon is recommending max sfm and for a 1/2" end mill, .007 cpt slotting and .008 for light peripheral. That's 420 ipm (slotting) on a 20k machine! Might be interesting to see what they'll really do but I do like their Ski-carb line. Have had good success with their (SGS makes a similar end mill) ski-carb 1/2" at max rpm and .006-.007 cpt, .125-.250 axial depth.

 

Chuck