View Full Version : Carbide question

loose nut
05-01-2008, 08:29 PM
I have always been told that carbide likes a good heavy cut at a fast feed and speed (This is a relative to the material being cut) and do not do well with interrupted cuts. With a lathe tool you can dig in and go but on an carbide end mill or face mill with anywhere from 1 to 8 or more inserts don't you have an interrupted cut on each insert per rev. What keeps the inserts from breaking down to fast or do they have a lower live expectancy then lathe carbide inserts.

mister honey
05-01-2008, 08:43 PM
Different grades of carbide are for different applications!

Milling grades of carbide are tough, tolerate interrupted cutting and thermal shock very well.

Turning grades are better suited to long, hot continuous cutting.

The amount of cobalt (the binder or glue in tungsten carbide inserts) reduces the wear resistance, but increases the toughness or strength.

That is, an insert with 10%-15% binder is tough, because there is more "glue" holding the particles of tungsten carbide together; but would wear quickly in a continuous cutting application.

An insert with 3% cobalt wears quite (in a continuous cut) well because there is less "glue" and more hard tungsten carbide in the matrix. However, it is fragile (in an interrupted cut) because the particles are not well bonded by the minimal amount of "glue."

There are other factors, too, but all carbide is not equal!


05-02-2008, 12:18 AM
All of my milling cutters are positive inserts. Even both my 6" shell mills. The inserts do not last long. My lathe inserts are negative and are tough as hell.
I do a lot of weld build up and turn it on the lathe. The carbide inserts last really well even with all the interupted cuts.
Heavy cuts... well I suppose. With razor sharp HSS I can wisk off .001 easy. With inserts I'm lucky to get .003 or so depending on the condition of the insert etc. A brand new edge will get me .002 for a bit. ,003 or ,004 is a safer bet as you never really know when you'll get .002.. at least on my sorta shaky 14X40.

05-02-2008, 01:53 PM
These days you can get really sharp carbide inserts like CCGT's that will make those superfine cuts. They'll take off "dust" if you want to.

These inserts look like this and are extreme positive rake:


That particular one is off a boring bar. The CCGT's will fit CCMT tooling.

Originally such inserts were for aluminum, but nowadays there are grades available for steel. They're not too happy with a really ugly interrupted cut--not sure I'd use them on a tough weld or some such--but they generally work really well. I keep this plus some regular CCMT's for the tougher roughing work.

A lot of folks will also keep an inexpensive diamond hone and use it to resharpen the edge of a slightly dull insert or brazed carbide tool.



05-02-2008, 01:56 PM
A lot of folks will also keep an inexpensive diamond hone and use it to resharpen the edge of a slightly dull insert or brazed carbide tool.

A diamond hone is also nice to take off the TiAN/TIN/TiACN coating from the insert. The coating is for high speeds and feeds, but it rounds off the sharp edge on the insert.

I try to buy uncoated inserts, which tend to be much sharper, but they seem to be pretty rare.

05-02-2008, 05:16 PM
I also really like the CCGT inserts that Bob posted above. I can grind a HSS bit fairly well. But those ccgt's work to good for me to mess with hss anymore unless I need a form tool. They work great even on my 100 year old Artisan, and VERY good on my SB9.They'll work just fine with the slower spindle speeds on the older machines. Best used for finishing and stick with the ccmt for roughing.

loose nut
05-02-2008, 11:47 PM
The 2" dia face mill I'm looking at uses TPG32* inserts, the same as used on lathes (the specs don't give the amount of binder in them) but it sounds as if they won't last long enough to make it worth the while, I might be better off sticking to HSS. end mills.

mister honey
05-03-2008, 08:37 AM
Is there a grade associated with or after the insert number: C2, C6, KC810, 883, GC4015, etc?


05-03-2008, 11:17 AM
The 2" dia face mill I'm looking at uses TPG32* inserts, the same as used on lathes

Most of those cheap TPG face mills have no axial or radial rake angle: the carbide insert sits flat in the pocket, and perpendicular to the shaft. Because there's no approach rake, they absolutely hammer the mill (which is really hard on the spindle bearings), and leaves a ratty finish.

I bought one of these when I didn't know any better, and it's now relegated to rough milling. See how the insert is flat against the pocket? The insert hits the workpiece flat and batters the machine. The TPG face mill in this picture is spinning at about 200 RPM:


The Dolfa and Grizzly TPG face mills are more expensive, but the pocket is angled with respect to the shaft, so like a helical mill, there's a gradual contact of the insert with the workpiece. So they don't hammer the machine, and are much smoother, and leave a much nicer finish.

This is one of my Sandvik RA-290 "shear mills" with high axial and radial rake angle. Look how the insert is tilted back in the pocket, and the pocket itself is angled backward with respect to the shaft. This type of face mill is made specifically for low horsepower, low rigidity machines, and leaves a mirror smooth finish:


loose nut
05-04-2008, 09:35 AM
Lazlo, I picked up a cheap one, 2" Dia. 3 inserts, for $29.00, just to try without spending a fortune if it didn't work out. On a piece of plate, 570 grade I think, at low speed you really get that thump, thump, thump that you mentioned, so I ramped the speed up to about 600 rpm's 0.025" DOC, just to see what would happen and the cutting smoothed out, the finish was a bit rough but my travel could have been a bit fast. After that I cranked the speed up to about 1300 rpm's and took a .005" finish cut with a slower feed and the finish was quite good for the type of material. The cuttings were not even turning blue at this tool loading. I know the rpm's were way to high but it seemed to work very well. If this works out I may get one of the face mills you mentioned but for hobby work I really don't need (want yes, need no) that kind of capacity.

05-04-2008, 12:54 PM

No, your rpms weren't too fast. At 1300 rpms, you would have been in the neighborhood for a 2" cutter. I regularly run a 4" with 8 TPG-432 inserts at 850rpms and depth of cuts to .700" in S7, D2, and 4140 steels. And no coolant. Insert life is good.

I suspect the reason why most people have a hard time getting good results with these cutters is they don't run them fast enough and hard enough.

So when you use that cutter, or most carbide insert shells, kick that pig! Don't be afraid to push it. That's what they need. And why they exist in the first place.


05-04-2008, 01:05 PM
So when you use that cutter, or most carbide insert shells, kick that pig! Don't be afraid to push it. That's what they need. And why they exist in the first place.


So what speeds and feeds should I run my 3" face mill with 4 cutters??



05-04-2008, 07:08 PM

A lot is going to depend on how rigid the setup, and how much HP is available at the spindle. So common sense and experience is needed.

But lets' use a standard BP type mill with 1 1/2 to 2 HP at the spindle, and a Kurt vice machining steel. As you found, your 2" cutter ran pretty good at 1300rpms. Depending on the material and depth of cut and feed rate, I would run between 1000 and 1500rpms. A roughing depth of maybe .100" with most BP's and a solid vice or clamped setup could run at 3" to 4" a minute in a face milling cut. You want faster feeds, reduce depth of cut until you achieve your desired feed rate.

A 3" cutter in steel, I run 800 to 1100rpms. You would want to probably lighten up your depth of cut to maybe .050" to .075" to maintain a 3" to 4" feed rate.

Thoughts to keep in mind. Tool steels generally "chip" better than mild steels, (mild steels can sometimes be "sticky" causing the chip to "smear" across the work surface leaving a poor finish), giving a better finish and tool life. Try to leave .030" to .050" for a finish cut. .005" finish cuts are hard on inserts. It causes heat build up and that accelerates wear on the edges. Always run as much feed rate as your set up will allow. You want a nice deep blue colored chip. Stay away from coated inserts in these cutters. They tend to "slap" harder than the shells with the higher rakes like the Sandvik that lazlo showed. Cheap plain ground inserts are best.

I wouldn't use this style of shell mill for aluminum unless it was all I had. They are really meant for steels and not "light" metals. Aluminum generally requires high shear angles to prevent edge build up and material welding. IF I was going to try it though, this might be the place to use a coated insert, (maybe TiN), I would maybe max out the rpms, use a light depth of cut, perhaps .025" to .050", and all the feed I could muster. But, I would expect problems.

------ Sorry, my train of thought is gone, on what I wanted to say. Was interrupted by an ambulance call.

Mostly the HSM suffers from two things with these cutters. Light weight, low HP machines, and an unwillingness to push the inserts hard enough.


05-04-2008, 08:14 PM
No, your rpms weren't too fast. At 1300 rpms, you would have been in the neighborhood for a 2" cutter.

A 2" cutter at 1300 RPM is around 700 surface feet per minute -- that's WAY too fast for a home-shop machine!

Mild steel is recommended at 130 - 180 surface feet per minute with a HSS insert, which is 250 - 350 RPM with a 2" facemill. You definitely want to be in that lower range for a low horsepower, low rigidity machine.

loose nut
05-04-2008, 09:21 PM
Now guys you have me all confused, is it to fast or to slow.:confused: :confused:



The first picture shows the new milling cutter, and unlike the one in Lazlos picture it has some rake although not as much as his more expensive face mill.
The second picture is a piece of boiler plate which I had handy and used as a quick test, It looks better in real life and it has a smooth to touch finish, a better piece or material would get better results.
The tooth drag as it follows around leaves slight uneven marks.

I know that carbide is suppose to be run hard but sometime I can get a better finish by taking a light cut at high RPM'S.

05-06-2008, 11:24 PM

Sorry it took so long to get back to this post. But, here is a Speeds and Feeds Chart that is pretty clear and easy to use. I've had this thing forever.

I hope you can see this clear enough.




I hope you can see that as the material gets harder, the cutting speed starts to drop. The soft steels that are typically used by most HSM has a face milling cutting speed of 560sfm to 725sfm. If we choose a start point of 600sfp, we would expect to run a 3" cutter at about 800rpms on a Bridgeport type machine. On your smaller, lower power benchtop type machine you can expect to run the same rpms, just not as deep a cut nor at the feed rate recommended. Running at too slow rpms is hard on the edges, (and your spindle bearings), because you get that pounding from trying to push the edge through the steel. Run at these faster rpms and that cheaper face mill will run smoother, sound sweeter, and the inserts will last longer.


05-07-2008, 12:07 AM
With all the different grades of carbide, you'd be better off looking up the manufacturer's spec on the carbide rather than relying on a chart from some other source. Some grades of carbide rely on very high temperatures to keep the pressure and shock of the tool entering and exiting the work down. Hard milling and high speed machining are two areas where this is evident. Other grades are for real heavy roughing in stuff like forgings with deep cracks and inclusions, and hardly handle heat better than HSS does.

If your mill can handle the speed and feed, then use it. My personal strategy is to continually bump the speed and feed of the cutter up until the machine starts to bitch about it. It is not possible to gauge the proper temperature via chip color when you use carbide. At work, on old clapped out bridgeports, one of the guys regularly runs a facemill so fast the chips come off bright red. The only way to really gauge carbide life is to actually look at wear vs. in^3 removed at different speeds. Thankfully, most manufacturers will supply you with a neato chart depicting this.

Carbide, in aluminum? How fast does your milling machine go? Keep bumping the speed and feed up (keeping the same chip load obviously) until the machine starts to not like it - same as steel. By limiting depth of cut to control power, most bridgeport-style machines can be run at the full 4000 rpm with a 4/5 tooth, 3" face mill. So just do whatever in aluminum. Watch the chips come off - if they all come off in one direction/stream without kicking the occasional chip off in an odd direction, you are running fast enough to not use coolant. If it kicks chips in different directions, go faster.

05-07-2008, 12:12 AM
Running at too slow rpms is hard on the edges, (and your spindle bearings), because you get that pounding from trying to push the edge through the steel.

Your Bridgeport speeds and feeds calculator shows the same SFM that I recommended: 160 - 200 SFM for HSS. A Bridgeport is way more rigid than a Mill/Drill, so like I said, 700 SFM is way too fast for a Home-shop machine.

In any event, the cheap TPG facemills hammer the machine because they're designed incorrectly (with a flat pocket), not because they're running too slow.

Picture standing in a pool, and align your hand parallel to the surface of the pool. Now slap the water.

Now angle the heel of your hand 15 with respect to the pool, and slap the water again -- your hand slices into the water because there's gradual contact. Now angle you hand 15 and your arm 10 -- your hand goes into the water even easier, because now it enters with a compound angle.

Almost all commerical milling cutters have axial and radial rake: the insert pocket is tilted backwards (positive rake) or forwards (negative rake), and the pocket is also angled with respect to the shaft (axial rake).

HSS endmills have axial and radial rake, for the exact same reason.

The Chicom TPG facemills are poorly designed, and they're hard on your machine at any RPM.

TPG inserts are pretty crappy to begin with, but if you really need a facemill with a cheap insert, at least buy the Grizzly or Dolfa versions, which correctly tilt the pockets so the inserts don't hit the workpiece flat.

By the way, the reason the thumping decreases at high RPM is because you're decreasing the DOC until you take a whisper-thin cut, and probably feeding very slowly as well, so you're spending most of the time cutting air and re-cutting swarf.

That's one way to reduce the hammering, but probably not the most productive way :)

loose nut
05-07-2008, 10:53 PM
I tried the carbide on aluminum and didn't like it, HSS gives a much better finish, at least on my machine.

The cutter that I bought does have a positive rake and cuts quite nicely if the speed is right, about 670 RPM'S (the next lowest speed is 345 and it hammers at that) on my machine, I only cranked the RPM'S up to 1180 RPM'S (not 1300, sorry my mistake) on the finish cut to keep the tool load up as the DOC was lower.

I'll have to do some experimenting to see what works best, but this is problematic because I mostly use Unknowium at home, what ever I can find cheap, for most none critical projects, the occasional car part for a friend is done with the proper materials but I don't use carbide on it anyway.

If all else fails it will be a roughing out tool and I'm only out $30.00 anyway.
Thanks guys.

05-07-2008, 11:48 PM
I have a HF-45 vertical mill - as many here will have.

Roughing cutters are my preferred cutter most times - does not hammer the machine, takes good speed and feed, works well on most metal that I use and gives "passable" finish although I often "finish-off" with and end mill.

These are of my insert cutter with positive rack and a scraper cutter insert:

These are cuts taken with the insert cutter on a disc brake drum going as fast as the machine would go and as fast as I could wind my 90:1 "Vertex" rotary table. I use the finished part to tram my mill.