How bout some speed feed help for some 60HRC steel?

[MetalFlake]

Happy Friday to the group!!

 

I'm going to have to skim cut (.005") from a case-hardened track. The stuff is 15-5. Do I treat it like inconel? Is there any tricks? I'll be using a 4flute solid carbide em (coated?).

 

Many thanks for any and all replies!!

 

Dan

[Hardmill]

Tialn coating would be best.

What are the capabilty of your machines??

A regular (geo) 4 flute mill will break down too

quick. Look at OSG exocarb-shp mills, reasonably

priced and very capable of doing the job.

A 10mm tool is in the 125-150 range.

I got more pricey suggestion if you need them.

With these tools you'll be in the 800sfm range.

Again it depends on your machine.

 

 

PEACE

[Fig sign]

Look also on Xpower from Y-G (Korea )

[T_MALENA]

Have any of you used tools from Tool Alliance? They are in California? They seem to work comparably to the OSG exocap shp.

 

I've used OSG Exocarb Max mills in 65-68 rc 12mm mill 525 rpm 4 ipm

 

Have used the OSG SHP mills in 55-60 rc 12mm mill

at 3500 rpm 38 ipm

[Thad]

I don't know what a 'track' is, but can you grind it?

 

If you only have to take off .005, I would imagine your average carbide end mill would do the trick. I don't know what 15-5 is either, so maybe I'm talking out my rear end.

 

Thad teh speak to me Oh toothless one

[g huns]

I use some of the OSG cutters mostly ball ends but I really like SGS cutters I get from MSC. 1/4 inch(that the biggest I can use in machine) 4 flute with corner radius TiAln, less than 25 bucks a pop. I cut 99% 54-56RC S-7, have cut 60RC D-2 with out to much trouble. When I first got this mill I burned up cutters like they were going out of style because I was going waaaaaaay to slow. Now I run 10k rpm and 250ipm with 1/4 cutter(HPPC on Fanuc control keeps her under control closer to 50 ipm average) cuts sweet. Also use alot of Niagara 2 flt when I can't have the corner radius, TiAln 1/4 in. about $10 each but don't last to long. Just give em to the boys running the bridgeports after I burn the corners off them, they think they're still brand new

[Thad]

Forgot to mention that we cut D2 (Rc 58-60) at 100-200 SFPM, .003-.005 chip load, and .02 depth of cut. If that means anything to you...

 

You certainly won't win any speed contests cutting like that, but the inserts last. General purpose insert, that is.

 

Thad

[TheePres]

15-5, a stainless steel used extensively by Boeing.

[?Mark]

quote:

---

I got more pricey suggestion if you need them.

With these tools you'll be in the 800sfm range.

Again it depends on your machine.

 

---

Hi Hardmill, now I understand your avatar

Willing to share those pricey options ?

Thinking about indexable Kennametal cutter with ceramic inserts but could use your advice on this.

I've got some A2 55-60 rc to face. Only about .005" but need a good finish on it.

 

Kind regards, Mark

[Hardmill]

For facing I'd go w/ Fette. They're an awesome

insert mill. I only use them for facing.

 

Kobelco are solid carbide and are now sold under

mitsubishi as miracle mills. Tough to beat this

tool. Got a tag to match too.

 

Hitachi is another great option.

 

PEACE

[?Mark]

Tnanks for a quick reply Hardmill.

Tried Fette few years back with not much luck above 55 hrc. I'll look at it again though, maybe they have better grade inserts than before.

Is 90 deg insert with about .005-.010" rad. what u have in mind? They are not that expensive.

I was quoted $80.00 per CBN insert for a mits cutter which I thought was way too high

 

Kind regards, Mark

[Hardmill]

You need the tialn coated inserts.

I'll be using that tool later this week. If I can

I'll shoot some video. What kind of machine are

we talking about??

 

 

PEACE

[?Mark]

It's a cat 50 mori vmc's.

No problems with rigidity and accuracy

 

Kind regards, Mark

[?Mark]

Just found this cutter and inserts(univex) in a tool crib.

These were regular ticn inserts so i guess that's where a difference is.

My, it's been 6 years since I used this cutter. Time goes by a bit too fast around here...

 

Thanks Hardmill, appreciate your input.

Here is to you buddy

 

Kind regards, Mark

[Hardmill]

Look on fettes' web site. I primarily use the

.5" , but they make a great 1" tool.

How big an area are you cutting??

 

PEACE

[?Mark]

The width of part is only 3/4", so 1" cutter will work great.

 

Kind regards, Mark

 

I'm browsing their web site as we speak...

[MetalFlake]

Thanks alot for all the killer input. Looks like I'll be going alot faster than I would have ever guessed...500sfm -wow- and a Tailn coating.

 

BTW this is a Boeing part 15-5 stainless. Only about 6" x 3" x .75" envelope in size and it's function is to guide a moving assembly along it's .500" wide track which is basically a 's' shape about 5" long.

 

Thanks again!

 

Dan

[Hardmill]

Along w/ machine and endmill, your toolpath is

equally important.

Let me know when you pick a tool and i'll help you out.

 

PEACE