[Swede]

I recently made my first foray into what might be called HSM. My little CNC mill has a KaVo spindle which can be run anywhere between 5K and 50K. Cutter was a 1/8", 4-flute uncoated microcarbide EM, new.

The material machined was fairly hard sheet carbon steel, 0.062" thick, unknown Rc but probably slightly harder than "spring" temper. The actual objects are Uzi submachine gun magazines which I am modifying to fit another firearm. The cuts consist of a simple rectangular clearance cut of 0.600" X 0.500" through the sheet steel, and a magazine catch slot of slightly smaller dimensions.

Here's what happened. I imported a DXF of the cuts and specified 0.015" Z step distance, 6 ipm feed. The best cutting action I obtained was at 12K RPM, but even then the cutter rapidly dulled. At slower RPM, around 8K, the cutter snapped. At higher RPM, around 15K, the chips came off sparking, it was ugly. In all cases, the cutter rapidly dulled and eventually broke. Coolant: I don't have flood yet; I was using hand applied tapmatic gold for lube. I broke or wore out 2 end mills to make only 12 cuts.

Am I WAY off here with speeds/feeds? Am I simply expecting too much from uncoated cutters through some fairly hard steel? Any thoughts and comments are really appreciated. This is new ground for me. I have experience with slower, manual machining.

Thanks fellas!:rainfro:

Oh yes, can anyone recommend software to determine speeds and feeds for this type of machining? I'm going to use primarily 1/8" and 3/16" carbide ball and normal end mills in a variety of materials with this spindle.

[Rekd]

Tialin Coated should work nicely dry. Not too expensive considering the life you'll get out of it.

Try smaller Z steps also.

'Rekd

[HuFlungDung]

Swede,

I would make sure that the endmill is being chucked quite short, in order to improve the stiffness of it. If you use an ER collet, you can actually chuck with some of the flute up inside the collet. This might improve the odds against premature breakage.

Use a light air blast. You don't want the tool stirring in a slurry of chips and a puddle of coolant.

The step-plunge motion maybe would be better replaced by ramping to depth. Does the part seem stiff enough when clamped for machining, or is there flex to it?

[Swede]

Thanks for the replies everyone. Rekd, I'll try various coated cutters. 99% of my previous machining is slow manual stuff and I have never needed the speed which makes coatings cost-advantageous.

Hu, I agree with you on the ramp to depth. This small run used a simple .DXF to G code conversion, which isn't sophisticated. The first cut was a straight plunge to 0.015" with a 4-flute mill, lots of nasty squall. That one plunge probably dulled that cutter instantly. After the first test cut, I edited the code so that the cutter plunged in air and approached the work on a horizontal plane. This worked better.

I think the answer might be as Rekd suggests, smaller Z steps and faster feed. By doing both, the cycle time shouldn't increase excessively. My whole machinist mindset is still geared to slow manual work with HSS, big feeds, slow speeds.

Funny, when I upgraded from a 3-1 mill machine to a BP clone, it took me a couple years to really understand how aggressively I could machine with the better mill. I was taking these goofy, wee cuts with the BP because I had been "burned" too many times with the 3-1 machine when I attempted to hurry things along.

Again, guys, thanks for all the expert advice. And I gotta ask again, can anyone recommend "speed/feed" software for this type of HS setup? Previously it was all an educated guess on my slow manual machines. I realize now that there is quite a bit of science behind optimizing an operation with a small, HS cutter.

[TAB]

I would suggest you talk to the tool reps. Many cutters and such will have very different operational paramters based on the geometry and coatings.

Kennametal is a good source of info. They have a good tech support line.

[Swede]

Thanks TAB.

Another question - coatings. I have a choice of TiN, TiCN, TiAln, ALTin. Of these, what would you guys recommend for general HS machining of steels, mild and moderately hardened? My copy of Machinery's handbook doesn't cover all of these. Again, thanks for letting me pick your brains.

[Ken_Shea]

Swede I asked the exact question to a carbide tool salesman. His statement, whether truth or fiction I cannot say, was that in most cases any of the coatings are better then none and while some coatings may be better suited to a particular task over another the decision on which one is mostly one of cost.

Ken

[arvidb]

Swede, according to my machinist's handbook, in steel you start to see the benefits of HSM at a "surface speed" or cutting speed of 500 m/min. Cutting forces gets significantly lower up to about 1000 m/min. Surface quality improves up to about 800 m/min, then stabilises.

This means that with a 1/8" cutter you'd have to run it at slightly above 50k RPM to start to see the benefits of HSM. The book also says that HSM in steel is difficult because of the lack of suitable tools and the very high spindle powers required. Ceramic or CBN (Cubic Boron Nitride) cutters is the most promising cutter materials (this book was printed in 2000).

Everything from the book, I have no experience whatsoever.

Arvid

[TAB]

Swede,

Whose tools are you looking at? The coatings are typically used to prevent the heat from attacking the carbide. Some offer abrasion resistance for materials which are abrasive.

If you have a catalog of the tooling vendor they usually have a chart with recommended speeds and feeds, DOC, and materials. I would consult those. I used to think the data was all BS and proaganda, but my experience in aerospace taught me that the manufacturers tested and created those parameters to help the end user. The paramters seemed vague and very general. This is due to the variety of equipment available and the variety of workholding set ups.

As for the ceramic and CBN materials, CBN is very expensive and usually used for very abrasive materials. Ceramic is awesome. It is very untolerant of vibration, and needs to run at a minimum of 900 SFM. usually, feed and spindle speeds limit the application of ceramics on anything less than high temp alloys. You could adjust DOC to get the 900 SFM but you might find that a little intimidating if the DOC is already farily heavy.