[DaOne]

I need some help! I have never cut steel before as we mostly cut aluminum. Now I need to cut out the same part in "Cold rolled steel" and I have no idea what to run my tooling at nor what depth of cut to take. To top it all off I will be using a new cutter that I have never used yet and really don't wanna break it by trial and error. The tools I will be using is... 1/2 4 flute carbide end mill, 1/4 4 flute carbide end mill and a (new tool)valentite 1 inch 2 flute carbide indexable cutter. basically I am looking for speeds and feeds to run these at in this material and attempt to make them simi efficient without killing the tools or myself . The machine I will be using is a Haas VF-2 with 7500 rpm spindle. I need to face the stock which I will use the valentite cutter. I also will be contour roughing it out using the same tool. Then finish using the 1/2 followed by the 1/4 end mills. Any help on this would be appreciated. Thanks in advance.

[laka]

Best place to look will be in the Valenite catalogue for the feeds and speeds for their tool. Just find the insert type and grade you are using and they will give you recommendations. Sometimes they feeds and speeds will be shown on the pack of inserts. Here is a link to their catalogue for milling.

http://www.valenite.com/internet/4558/Internet/Global/S000985.NSF/LookPortal/Portal9CA1F1642FD8AC128525748F005F7308/$FILE/ValMILL_Catalog_2007.zip

You should also be able to find some cutting parameters for the endmills in there also. Cold rolled steel is quite easy to machine. Your machine won't have any problems.

Good luck

[KLUCAS4]

Well For the Carbide Endmills on steel use about 300 SFM on Alum This would be about 1000 SFM. A simple formula is SFM X 3.82 / the Dia. Of the Endmill. This will give you your RPM's. Then Multiply that by the number of teeth of the endmill for example.

300 X 3.82 = 1146 /.25 (dia. of endmill) = 4584 RPM's
4584 *.004 = F18.336 would be the feed @ .001 Per tooth per Rev. ( 4 flute endmill)

If I am understandning you right the endmills are just for finishing so depending on the finish you are looking for you probably could run this faster. I am just trying to give you a safe starting point.

As far as the 1.0 indexable rougher I uasually run mine at 400 SFM On Steel @ 25 IPM with a .125 Depth of cut. And thats probably mild compared to most. I have a iscar with 3 inserts and a ingersol with 2 inserts. If you take .062 you probably could ramp this up.

[dynosor]

High rotational speeds will chip a carbide endmill cutting steel regardless of load per tooth. 2500 RPM for the 1/4" cutter and 1250 for the 1/2" cutter should be OK for mild or annealed steel - go lower for harder materials.

I suggest reducing the speeds, feeds and depth of cut used for aluminum by a factor of three to start.

[Geof]

dynosor's suggestion to use one third the sfm that would be used for aluminum is pretty good, but don't reduce the chipload by the same amount; on cutters larger than 3/8" you can keep the same chipload as for aluminum at around .5% to 1% of the tool diameter.

Using multiflute cutters I think it is best to use coolant but with the insert tool the best results may be obtained using air blast and keeping the sfm up around 400feet per minute with a chipload of about 0.005" up to 0.015" per tooth at a depth anywhere up to .20" or even more.

With the insert cutter running under optimum conditions the chips should be comming off blue colored but the cutter and the workpiece should remain cool enough to touch. The idea is to have a largish chip coming off quick so the heat of cutting remains in the chip not transferred to the tool.

[DaOne]

I tried a sfm for the 1 inch insert cutter of 400 (1528 RPM / 15 IPM) and it sounded horrible. Sounded like it needed to go faster on the rpm? There was allot of chatter. Any Ideas?

[dertsap]

if youve got chatter at such a low sfm , either your holder is no good , your cut is too heavy or the part isn't very rigid
on a decent insert mill with the proper inserts i wouldn't even consider running it less than 1200sfm on mild steel , for eg. i used to use the sandviks , we had a number of parts that were 1018 that we cut with a 3/4" dia at .1 to .125 depth @1400 sfm minimum , insert life was incredible , the load was nearly nothing and it sounded beautiful

right now you are running the insert at the minimum chip load , you may have better luck to feed a little heavier

[DaOne]

OK, turns out the tool I have only cuts with one of the two flutes. The other flute is only used for plunging. So being its a single flute (something I have never used) I tried 500 sfm (1910 RPM and 10 IPM) at .1 depth of cut for roughing and the cutter lasted 3 parts and broke a carbide. I am using flood coolant on a Haas VF-2

Here is the tool I am using...
http://www1.mscdirect.com/CGI/NNSRIT...MT4NO=55314826


and here is the insert I am using...
http://www1.mscdirect.com/CGI/GSDRVS...00000078732720

[little bubba]

You just learned what the definition of thermal shock is. From back when running dry scared the everliving bejeezers out of me, because it just seemed wrong, I found that the "magic" # was about 280sfm for carbide, milling in mild steel, above that with decent flood coolant, tools bit it pretty quick.

Thermal shock, well, carbide can take heat, tons and tons and tons and tons of heat. It can not take thermal cycling. You were cycling that carbide from well over 1000 degrees(locally) to coolant temperature 1900 times a minute.

Derstap said 1100 sfm on the indexables, I agree, really conservative on the indexables, 600sfm. 1100 is the high end of comfy, 1400 getting after it and upwards of 2000sfm when taking a finish cut or just dusting off the top.

Solid carbides, I assume you bought some coated variflutes or roughers (square corner finishers are for finishing period). On a full slot, 425sfm to be conservative but effective. I find 500sfm to give very good tool life in 1018. When running narrow and deep (chip thinning) up to 900+ sfm. Dry, and air blast when chips need to be cleared, but most of the time they are flying and clear themselves.

I'm guessing you are running about a 15hp machine, a good 1/2" endmill will move enough metal to bring your spindle to a halt.

Also, remember that a TiAlN or AlTiN coating starts working its magic around 1700 degrees F, so coolant is not your friend here, or the carbides friend.

Remember a TiAlN or AlTiN coating starts working its magic around 1700 degrees F, so coolant is just going to kill you.

[dertsap]

On a full slot, 425sfm to be conservative but effective. I find 500sfm to give very good tool life in 1018. When running narrow and deep (chip thinning) up to 900+ sfm. .

425 is definitely conservative for a good variable mill , the Gorilla Mill slotting mills that i distribute should run at 600 sfm for full slotting on mild steel , full slotting with these mills is 2 x dia

[DaOne]

So what should I try next? Same speeds and feeds and depth of cut just without coolant? how would you guys run this cutter. I can post my part file in mastercam if that helps.

[dertsap]

your best bet is to find the manufacturer specs for side milling with that tool , i hadn't realized that was a plunge mill until just now , i would imagine that its side milling will be fairly limited but i could be wrong , a valinite rep would be able to recommend speeds and feeds which would best suit you , an email is a painless way to get 100% good info . i have very little experience with the plunge mills and i would hate to steer you wrong any further than i may have

[dertsap]

http://ftp.cnchungary.com/Varsanyi_P...ok/milling.pdf

it say 200-450 sfm , 4-10 ipm

internet ! gotta love it

[DaOne]

Ok, turns out the tool we got is actually defective. They are giving us a full credit and told us we can get something else or the same tool. Can anyone recommend one for what I am doing. Basically I am taking a skim pass to surface the steel. Then I am roughing it out removing all the material I can as fast as I can. Then I will be finishing it with a 4 flute 1/2 cutter. next a 1/4 4 flute cutter. I would like a indexable cutter for this so I can use it for aluminum down the road. Preferably 1 inch in diameter. I don't need it to plunge. The cutter needs to be sold at MSC.

http://www1.mscdirect.com/cgi/nnsrhm

[dertsap]

it seems they sell ingersol , look for a 1" that uses the apkt inserts , i didnt see it on the site but i didnt search for it either , ingersol makes a good mill , better yet is if you can find a sandvik with the same insert style

[DaOne]

Since this is kinda a 1 time deal (cutting steel parts) and I am making 130 parts I don't need a top quality tool. I just cant replace a $15 carbide insert after 3 parts. The tool I was looking at was this.

http://www1.mscdirect.com/CGI/GSDRVS...00000078888596

Do you think this is ok or should I look for something that takes the apkt inserts?

[ALLtra Mach]

Not familiar with your machine or why your using such a small mill.
But if your end milling, you can rarely go wrong with the APKT tools. They do great side work, and can face too.
I'll argue SECO over Ingersoll all day long, but thats not what your asking LOL.
The APKT has become popular. And are available in generic cutters.

Item #67926220 Is a Seco Mill $280
Item #80608870 Is a Hertel $270, c0omes with 10 inserts.

So you can save $100 using the cheaper tool, HOWEVER.
You will soon learn to love this tool and use it constatntly. I haver them in 6 sizes from 3/4 to 4".
The tool life you will get out of the Seco is 40% to 50% higher, and the cost savings in just a few months will justify the extra initial invest ment.

Ingersoll,ISCAR, Kennametal, Sandvic...all the majors make one of these mills. Pick your favorite.

[DaOne]

Ok, I am able to get a deal on a Iscar cutter. I can get it in 2 or 3 flute. Whats best for steel? Now I see the APKT cutters come in different types. I am looking at the 1003 and the 1604 types. What would be best for this application? Also what grade would you recommend?

[DaOne]

Appears like I am looking for a 1003 style insert with a grade of IC520M. I just wanted to be 100% sure before I give the go ahead on this. Now I just need to know if I should do 2 or 3 flutes on steel?

http://www.iscar.com/Ecat/familyhdr....lang/EN/type/1

[ALLtra Mach]

In 1" I use a 3 flute, any smaller go with 2 as chip clearance starts getting small.
However, If you decide to ever use it on aluminum you'll want the 2 flute, though the 3 would work.
So your choices are;
2 flute, Less productive in steel, more productive in aluminum.
3 flute, less productive in aluminum, more productuive in steel.

So it is simply what will you use more of it for?

As far as grades and styles, If your getting this from MSC, they have excellent tech. Call them with your application and they will get you what you need.

[email protected]

This is my rep for them, Great guy, very helpful.

Tell Him Jon from Alltra said he'll take good care of you!