Use and care of a 3/4" carbide insert cutter

[PixMan]

Ok members, so I had an hour or so to kill in the shop today and since I received ten new inserts I'd bought off eBay yesterday. These "steel grade" inserts were in addition to the ten "aluminum" grade I'd got a few days ago.

What I thought to do here was to lay out step by step the proper way to use carbide insert tooling in a milling machine. This applies primarily to those with a range of spindle speeds and programmable (or at least, selectable) feed rates. It's what any programmer or operator in a commercial shop should be doing; using the resources provided by the manufacturer of the tools to get the most out of them. Unfortunately, few if any other makers besides Walter really bother to put ACCURATE, RELIABLE data in their catalogs. That said, you should be able to do this with any make of tooling and get acceptable results.

First order of business, identify the material to be cut. In this case, I will be using AISI 1018 cold rolled steel. It's about 0.18" carbon, and runs about 125 Brinell hardness.

From the Walter catalog, look up the cutter first, then insert grade to be applied. in this case, I've chosen my 3/4" F4042R cutter and ADMT10T3PER-F56 inserts in grade WKP35S.

Here's the new ADMT (as molded, not ground) insert next to an ADHT10T3PER-G88 WK10 insert. Steel likes a more honed edge for high material removal rates, unlike aluminum.


Now I look up cutting speed in surface feet per minute (or meters per minute if working in metric. From the Walter catalog, I look at the "blue" pages for the "P" class of steels, which is all your carbon steels as well as ferritic/martensitic stainless. Here we see for "1/1" (cutting width at full diameter of cutter), the 690 SFM. Note how the speeds can rise fast as cutter engagement is less. Also note how the preferred method is "coolant off" for steels, shown by 2 dots for faucet "x'ed" but only one dot for faucet on.


Now to covert to RPM, as my machine is a manual spindle and not smart enough to take speeds in SFM. It's simple mathematics.


The bottom formula is the one most people use. I do everything the hard way.

Now armed with an RPM and cutting speed, I need the feed rate per tooth so I can get "inches per minute" on the feed unit (manual machine with feed) or CNC control. That's in the Walter catalog too, just a couple pages beyond the cutting speed charts.


Now I can calculate feed rate in inches per minute. I am spinning at 3514 rpm. Multiply that by the .007 inch per tooth, times the 3 inserts in the cutter. I round it down to 3500 rpm, the closest index mark on my spindle speed chart.

3500 x .007 x 3 = 73.5 inches per minute feed rate. On my particular machine I have power feed at 80ipm or 60ipm. Better I back down. I also want to know how much power I can expect to use for a given cut. With the Walter Machining Calculator on my Android tablet, I can get the load if I look up the rake angle of the insert. That's also right there in the Walter catalog! It's 16º for my new inserts.

 

At the original speed, feed and a .050 depth of cut at full .750" width, it would pull over 2.8HP and probably stall my machine, so says the app.


Correcting to the 60 inch per minute feed rate I can do, I'm backing off feed to .0057" per tooth. Here's the results with corrected parameters.
It shows just about 2HP, and I am willing to take a chance. Bear in mind that it's a 2HP cut but a belt drive spindle. I'm counting on sharp new inserts, soft steel, rigid setup and luck.

[PixMan]

Well this is the Walter Machining Calculator output.


And this is what a 6-1/2" long cut at 3/4" wide and .050" deep looks like in 1018 steel at 3500rpm and 60 inches per minute:





The chips it made landed a few feet away from the machine. Not heavy, but hot and fairly sharp. I couldn't actually find any on the machine! You can hear the spindle work when it enters the cut and unload as it exits.

This is what the inserts look like, just some of the rust from the stock on them. I'm certain I could get at least 30-40 minutes of cut time per edge under those conditions, at a minimum.


The finish is shiny but probably about a 32-40Ra (microinch). It could be smoother at a lower feed rate, but probably wouldn't be as "shiny" from the heat of the process.


Any questions?

[EdK]

Holy crap that mill is moving, and climb milling at that.
Thanks for posting that.

Ed

[PixMan]

Actually Ed, it's really not climb milling. When you go full width, or really anything beyond 1/2 the cutter, it's neither climb nor conventional in the pure sense. It's just plain ol' milling.

[EdK]

(11-16-2014, 07:13 PM)PixMan Wrote: Actually Ed, it's really not climb milling. When you go full width, or really anything beyond 1/2 the cutter, it's neither climb nor conventional in the pure sense. It's just plain ol' milling.

Ok, that makes sense.

Ed

[Mayhem]

(11-16-2014, 06:55 PM)EdK Wrote: Holy crap that mill is moving...

I thought he had hit the rapid traverse button!

[PixMan]

Nah, that's only 60ipm. Rapid traverse on my machine happens to also be the maximum feed rate of 99 ipm.

My point with this isn't to show how fast my machine goes, but to show how to arrive at the recommended speeds and feeds. You can always back it down from there, but when you do I think the most important thing is to keep the carbide doing some work in feed per tooth. As soon as you back off on feed rate, you'll rub the insert to death.

If concerned about chips flying and wearing out inserts, lower the cutting speed and just keep the feed rate commensurate. Don't go too low on cutting speed, you'll break the carbide. However, once you get down to 100 surface feet per minute, why bother with carbide insert tools? You might as well wear out some HSS.

P.S. - This cutter works just SO much better than the Kennametal one it replaced it's ridiculous!

[Mayhem]

I was just teasing

The sad thing is that in your shop it all (sort of) makes sense but then I get home and see these posts and then feel dumber than a box of hammers trying to keep up. I'm sure it will make much more sense and stick in my head once I get my mill up and running...

[PixMan]

(11-17-2014, 08:23 AM)Mayhem Wrote: I was just teasing

The sad thing is that in your shop it all (sort of) makes sense but then I get home and see these posts and then feel dumber than a box of hammers trying to keep up.  I'm sure it will make much more sense and stick in my head once I get my mill up and running...

You don't give yourself enough credit Darren!

When you were here you did just fine with my machine, and with practice on yours you'll be flying.

[mike-sid]

Great post and info on selecting speeds and feeds for carbide tooling! That really made a nice cut, love the video. You are full of info on carbide inserts and always willing to share. Just last night I was reading through my notebook of some of the information you taught me. Thanks!