Mills. Is there a time HSS is better than carbide?

Hi all,

Ran into a problem a few nights ago while trying to finish a job and being new to this, it seemed strange but after thinking about it maybe it's not so weird.

I'd like some thoughts on it.

We were milling a slot clean through some 1/8" aluminum angle. The easiest way was to clamp the angle in a vice with the other side hanging horizontal over the vice. We then just milled our slot through it with a 1/4" square end mill.

We were running 30 inches a minute @ 5000 rpm using a 2 flute HSS 1/4" mill with 3/8" shank. This worked beautifully, good finish, not much noise etc.

I decided to swap in a solid carbide 1/4" 3 flute endmill and the results were terrible. A lot of noise and chatter and the finish was terrible. Figured maybe going to a 2 flute would fix it, but the 2 flute carbide mill had the same problem. Going back to HSS solved it.

I'm assuming the cause of this was the material wasn't terribly rigid the way we were holding it and the carbide simply didn't get along with that scenario. The carbide mills were a little longer than the HSS, but not a huge amount, I think the carbide's flutes were 1/8" longer.

We did almost 200 pieces with the HSS mill and no problems.

Thoughts? Are there times HSS is preferred over carbide from a performance standpoint?

it just sounds more like your carbide end mills were pieces of shit.

Larry Dickman said:

it just sounds more like your carbide end mills were pieces of shit.

Click to expand...

"UltraTool made in USA".

It's possible I suppose.

What's your go to brand? How is Lakeshore Carbide or HTC?

I think your scenario is one of those occasions when the set up rigidity, material type etc does lend itself to a HSS endmill. Its not so much the HSS being "better" than carbide. Its really because the carbide would probably run around 15K RPM in aluminum which would create harmonics, tool pressure etc. with the setup you have. I have ran into similar things at times. I know if I am cutting something in a less than kosher manner HSS will be more forgiving than carbide. When a carbide endmill would chip.....sometimes a HSS wont.
Side note......3 flute endmills work great for slotting. It was the cutting parameters and set up holding it back. HSS endmills also tend to have a sharper cutting edge.....

Yes, HSS is often more tolerant of dodgy setups like you describe. Carbide is extremely stiff and brittle. It will break long before it will bend. HSS can take a lot of punishment before it breaks.

This is one of the reasons manual machinists don't trust carbide drills. They need a rigid setup and controlled feed or they shatter into a million expensive pieces.

Larry Dickman said:

it just sounds more like your carbide end mills were pieces of shit.

Click to expand...

With the tuning-fork of unsupported overhang in a clamping arrangement that s****y?

He should mayhap be using a sawdust-maker's router @ 15-20 K RPM so as to sneak-up on the shiney-wood FAST and pierce if before it even knows it is being f****d-with. It won't have TIME to vibrate...

I almost never use carbide on anything, but I don't do production work. HSS, especially the HSS with cobalt alloys are superior in both lathe and mill work when doing one off or maintenance type work. They are sharper and tolerate more rake than carbide, plus they like lower speed cutting. Carbide tools require much higher speeds, stiffer setups and more horse power, which are great for long CNC production runs, but not so much for job shop applications. That's not even mentioning lower cost.

steve-l said:

I almost never use carbide on anything, but I don't do production work. HSS, especially the HSS with cobalt alloys are superior in both lathe and mill work when doing one off or maintenance type work. They are sharper and tolerate more rake than carbide, plus they like lower speed cutting. Carbide tools require much higher speeds, stiffer setups and more horse power, which are great for long CNC production runs, but not so much for job shop applications. That's not even mentioning lower cost.

Click to expand...

I don't think I have even a single power-saw blade or router-bit left in my sawdust-making arsenal that is NOT Carbide. Drills can be HCS or HSS, but not the saws.

Shiney-wood gets worked with those wood tools, too, of course. Doesn't need nor deserve anything else.

Masonry drills are Carbide, but tips only. The tile "wet" saw has a diamond blade

Other side of the wall, where REAL metals - CI, steels, and the Bronzes - are worked, it's the other way 'round. HSS, HSS-Cobalt, even HCS. Hardly ANY carbides, save the odd solid carbide "problem solver" drill or shapeable Carbolly brazed-on set aside.

steve-l said:

I almost never use carbide on anything, but I don't do production work. HSS, especially the HSS with cobalt alloys are superior in both lathe and mill work when doing one off or maintenance type work. They are sharper and tolerate more rake than carbide, plus they like lower speed cutting. Carbide tools require much higher speeds, stiffer setups and more horse power, which are great for long CNC production runs, but not so much for job shop applications. That's not even mentioning lower cost.

Click to expand...

Interesting.
I did not know HSS tools were sharper than carbide.

Our machine is 7.5HP but only spins up to 5000 rpm and we are a job shop, don't usually do a lot of high quantities. The machine works great with steel, stainless etc but seems to be on the slow side for aluminum.

It sounds like HSS is what I should be buying in general.

cj133 said:

Interesting.
I did not know HSS tools were sharper than carbide.

Click to expand...

They CAN be. Or become dull.

Large or complex ones may be worth periodic sharpening fees. Small ones are usually cheaper to replace.

Our machine is 7.5HP but only spins up to 5000 rpm and we are a job shop, don't usually do a lot of high quantities.

It sounds like HSS is what I should be buying in general.

Click to expand...

Face or shell mills and lathe tooling, Carbides probably make better sense - especially if you have weld build-up to cut back or have to work hardened steels w/o annealing.

Drills or end mills? HSS when you can, Carbide when you must.

And cheap s**t that doesn't hold true to proper size, strength, shape, edge geometry and sharpness? Never. For either.

It will take your money, irritate your ass, f**k with your mind, waste your time, and annoy any pig within earshot.

Monarchist said:

They CAN be. Or become dull.

Large or complex ones may be worth periodic sharpening fees. Small ones are usually cheaper to replace.



Face or shell mills and lathe tooling, Carbides probably make better sense - especially if you have weld build-up to cut back or have to work hardened steels w/o annealing.

Drills or end mills? HSS when you can, Carbide when you must.

Click to expand...

I realize our setup wasn't the best, but it got the job done fast and worked well with the HSS mill. It just seemed strange to me that when I tried using what I believed to be a better tool, the setup completely failed to work while the cheaper HSS had absolutely no problems.

Like I said, I'm new to this and I've got plenty to learn, that's for sure.

cj133 said:

Our machine is 7.5HP but only spins up to 5000 rpm

Click to expand...

Therein lies the problem with carbide. Your were running@ 312 SFM with HSS which is about right.Way to slow for carbide.
For machining aluminum, I like 2 flute, hi helix, HSS endmills. They just work good on a machine with limited RPM.
JR

There are plenty of guys here that know more about tool geometry than I do. HSS doesnt have the edge prep that is given to most carbide tools. Without the edge prep carbide would chip easier than it already does.

Ok, so I've been trying carbide from time to time, and it's still failing for me.

Yesterday, I needed to mill a 9" x 9" x 1.5" thick hot rolled steel plate. We already milled the black surface off of it, so it was just clean silver steel on all sides.
I clamped it in a Kurt 6" vice extremely tight. Using a 1/2" 4 flute carbide endmill with 1" flute length in a new ER32 collet torqued to spec I ran 2600 RPM and it still screamed and chipped the hell out of the mill.

HSMAdvisor recommended something like 3000 RPM @ 30 IPM, but I started out slow and the highest I felt safe at was 10 IPM. Dropping the RPM to 2600 helped, but it still ruined the mill.

I'm using flood coolant as fast as I can on an open machine without getting a shower.

Once again, switching to an HSS mill solved the issues. It ran nice and quiet and left a beautiful finish.

What am I doing wrong?

Things that I wonder which very well could be totally irrelevant are.

Is the issue I'm going too slow? That doesn't seem likly as the faster I go, the louder it gets.

The spindle on this machine is belt driven, can that cause issues?

What about slop in the spindle? It seems to mill accurately within 0.001, but could there still be enough wear on the machine to cause problems?


I'm just confused how some guys can apparently cut at 30 inches per minute using carbide while I'm stuck at 5-6 IPM with HSS.
I'm assuming it's something I'm doing. But what?

you can go slow rpm with carbide i do it all the time as most tool in tool holder setups on particular parts have a max rpm (sfpm) when vibration becomes a problem.
.
many a time i have gone faster by going slower
.
with aluminum hss often is more than fast enough

cj133 said:

I'm using flood coolant as fast as I can on an open machine without getting a shower.

Click to expand...

Carbide doesn't tolerate thermal shock well. It's heating up through the cut and then immediately cooling down once it hits coolant. This heat-quench cycle causes chipping. Try the same parameters with air blast to clear chips and prevent re-cutting. This style of machining (dry cut with air blast) works best with a coated tool, usually AlTiN or some equivalent. The coating gets super slippery at high temperatures and thus allows better chip flow.

Also, as others have mentioned, carbide works better with a rigid setup and rigid machine. What, exactly, were you running this job in? From what you said (7.5HP, 5k RPM max, belt-driven), it doesn't seem to be a machine that'll take kindly to the newest recommendations on tooling feeds and speeds?

mountie said:

Carbide doesn't tolerate thermal shock well. It's heating up through the cut and then immediately cooling down once it hits coolant. This heat-quench cycle causes chipping. Try the same parameters with air blast to clear chips and prevent re-cutting. This style of machining (dry cut with air blast) works best with a coated tool, usually AlTiN or some equivalent. The coating gets super slippery at high temperatures and thus allows better chip flow.

Also, as others have mentioned, carbide works better with a rigid setup and rigid machine. What, exactly, were you running this job in? From what you said (7.5HP, 5k RPM max, belt-driven), it doesn't seem to be a machine that'll take kindly to the newest recommendations on tooling feeds and speeds?

Click to expand...

.
aluminum has a nasty habit of sticking to flutes when milling dry

At work it's all manual machines. Carbide is used on the lathes. On mills its mostly HSS roughers, and a carbide insert flycutter.

Carbide spade drills are used for the big drilling, they seem to take some real abuse. But HSS for stuff under 1/2" or so.

HSS roughers, even when they look like they are dead, seem to keep cutting on worn machines in nasty materials and goofy setups.

I personally don't use much carbide on my machines. But that's mostly because the heavy rigud machines arent runing yet. When they come back to life, ill probably get some carbide tools.

mountie said:

Carbide doesn't tolerate thermal shock well. It's heating up through the cut and then immediately cooling down once it hits coolant. This heat-quench cycle causes chipping. Try the same parameters with air blast to clear chips and prevent re-cutting. This style of machining (dry cut with air blast) works best with a coated tool, usually AlTiN or some equivalent. The coating gets super slippery at high temperatures and thus allows better chip flow.

Also, as others have mentioned, carbide works better with a rigid setup and rigid machine. What, exactly, were you running this job in? From what you said (7.5HP, 5k RPM max, belt-driven), it doesn't seem to be a machine that'll take kindly to the newest recommendations on tooling feeds and speeds?

Click to expand...

The machine is a South Western Prototrak SMX FHM7 from I think 2008. They still make the same machine with minor changes I believe.

Here's a link to the machine and the current specs.
Southwestern Industries, Inc.

DMF_TomB said:

.
aluminum has a nasty habit of sticking to flutes when milling dry

Click to expand...

Depends on how fast you are going.. Those Korloy ripper mills.. Going at 6061 DRY...
That was scary the first time I hit the big green button. Just polished carbide, no
coating.. If you go at it WET, you run into that thermal shock thing and the inserts
chip out, DRY, they last forever.

That was THE MOST SCARY green button push I've done in my life.. I hit the button, and I RAN..
And it just cut and cut and cut and cut.. Running 2000+ SFM, and over .020" a tooth.

Back to the OP's problem.. What exactly is a "4 flute carbide endmill".. Is it a square corner,
un-coated, 90-90-90-90 endmill??? The cheapest thing you could buy??? I bought 4 of them 9 years
ago to have on hand for finishers, 2 of them are still in the packaging. Coated variflute/helix,
with a corner radius.. They cost a bit more, but they are worth it in every way...

Also, why an ER32??? I find they just compound problems.. All kinds of bits and pieces and interfaces
that can move and shift.. Set screw holder.. About the simplest, cheapest holder in the world, and that
doesn't mean they are bad...

And then the coolant thing that has already been mentioned.. I found the cut off from Dry to Wet is around
300sfm in mild steel.. Under 300 and you're fine running wet.. Over 300 or so and you start running into
that thermal shock problem. As for air blast, if your chips are getting themselves out of the way, then I
don't find it necessary.

And don't be AFRAID to run dry.. Up above I told you about the scariest green button push of my life.. Well
the second scariest was the first time I tried one of those fancy Variflute Endmills... 2005 or 2006 or so..
It was a 1/2" HTC (before Maritool sold them).. 400sfm DRY, full slot, right into a block of 4140..

Its not going to work.. It CAN'T work.. How can you cut STEEL with no coolant, at those kinds of speeds??

My butthole was all puckered up.. AND IT WORKED!!!! IT WAS AWESOME!!! I called over an old school grouchy
guy that worked for me, and he said "That's not bad for aluminum".. Its not aluminum!!!!

That day changed my life.