Carbide endmills Aluminum vs non-aluminum ???

[zaebis]

Folks,

Those who have used lots of so called aluminum endmills (35 heliz + peculiar tip) vs traditional 30 helix of the same size. Is there really a difference for aluminum applications?

[Geof]

Better chip clearance during aggressive metal removal at high speeds, chipload and depth of cut.

I think that is about it.

Aggressive as in 3/4" two flute at 11,000 rpm, full width, 0.4" deep and 120 ipm feed in 6061 with flood coolant.

[zaebis]

Originally Posted by Geof Better chip clearance during aggressive metal removal at high speeds, chipload and depth of cut. I think that is about it. Aggressive as in 3/4" two flute at 11,000 rpm, full width, 0.4" deep and 120 ipm feed in 6061 with flood coolant.

So you have better finishes? Could you not feed like that 30 degree general purpose carbide 2 fluter?

[Geof]

Originally Posted by zaebis So you have better finishes? Could you not feed like that 30 degree general purpose carbide 2 fluter?

I din not mention anything about finish just metal removal during a roughing operation; this is when the high helix cutters with deeper flutes for better chip evacuation often perform better than a general purpose cutter. The helix tends to lift the chips out of the cut better.

Regarding finishes there is not much difference but many of the 'aluminum' end mills are made from micrograin carbide so they have a much keener cutting edge, this can give a better finish especially at high surface speeds.

[dertsap]

Originally Posted by zaebis So you have better finishes? Could you not feed like that 30 degree general purpose carbide 2 fluter?

35-45 deg are ok but if you go up around 55 deg then the 55 deg high helix has more shear to it which will provide a better finish

[moldmaker5]

I have become a firm believer in specifically designed endmills. I have been using New-Tec’s 45-degree aluminum finishers and have been getting mirror finishes in 6061 & 2024 for 7 years. Many of the purpose made endmills have wiper lands and other such features.

Ditto on dertsap's post. I have a friend who uses 60 degree endmills in making tapered aircraft parts 2"x12"x.1" the middle tapering down to .040 at the ends and held down only on the ends (2" dimension in Z, 12" in X, clamped against a plate). Any other endmill rips the part out. In his case he uses an inexpensive Taiwan made 60 degree .5" 3 fluter. As the grinding isn’t near as nice as on the carbide stuff we figure it must be the shear angle.

An endmill engineer once told me that if the same cutting edge is engaged in the cut in two places at once (like what you would get with a long 60 degree endmill) the harmonics do bad things-that’s why they don’t offer 60s anymore.

[Shotout]

Originally Posted by zaebis Folks, Those who have used lots of so called aluminum endmills (35 heliz + peculiar tip) vs traditional 30 helix of the same size. Is there really a difference for aluminum applications?

I'm pretty fond of the Accupro (MSC) 3 flute 35deg helix ZrN coated endmills in aluminum but have recently started using the same spec Titan end mills with the same results. These aluminum specific end mills are worth the price over more conventional 2 flute end mills as they allow you to remove metal much more efficiently, meaning better profits. I have a job on one of the mills at work right now that runs a 3/4in .06R bull mill at 9600 rpm; 415ipm with a .245 DOC and a .450 step over. 40 taper 15K spindle using the high speed machining control parameters with a constant spindle load of 93% with a couple of entries into "heavy" corners that spike up almost to 130% for 5 or 6 seconds. If this was a conventional end mill I'd be running around 100-130ipm. This mill is finishing some features of the part feeding at 215ipm leaving better than a 125 finish which is within spec. If the surface roughness call out was tighter I'd run it at about 8600 rpm feeding @ 93ipm on the finish passes to hold a 63 roughness walls and floors. Tool life is good, roughing 6 parts with a cycle time for that tool of 35 minutes. With machine time @ $75US we are more than paying for the extra end mills and making more money per part than a more conventional end mill would allow. The only draw back was the operator kept calling from the floor on the first part to tell me I was running the tool entirely to fast. I finally took him a roll of toilet paper and told him 3 squares only per part. After that he cut one complete part and saw the condition of the tool. He was then bragging to the other operators about what he was doing on his machine. I am cutting 7075-6 but proofed this in 6061-6 plate we cut on the waterjet. In 6061 the spindle loading was slightly lower and the chip a little tighter but otherwise the same. The difference for me is profits for the company and moving more part numbers across my machine table.

[John Welden]

Best thing you can do is go for 3 flute instead of 2. Huge improvement.