[SCzEngrgGroup]

Incidentally: Back when I was actually running the part in question using the HSM tool paths I'd generated, I deliberately measured the thickness of several of the Metal Shavings that flew off of my metal stock. Out of curiosity, I wanted to see if they were actually .015" thick. I did it sort of haphazardly; putting my digital calipers on what I thought was the thinest part of the shavings. The thickness of the few shavings I measured averaged close to the .015" that they were supposed to be at. Looking at these metal shavings with the naked eye, you can see that they don't come off the metal stock as a flat shaving. They're more of a pig-tail shaped shaving. I mention this because even though I tried to measure thickness at the flattest points of the shavings, inevitably I'd get measurements thicker than .015".

Width of cut is only vaguely loosely to chip thickness. Actual chip thickness will almost never be equal to WOC, and can be much greater, or much less, depending on the cut. Chip thickness is a function of many complex factors, but the dominant factors are RPM and feedrate, not WOC.

Proper feeds and speeds calculations, especially for HSM, is a VERY complex subject. That's why you'd be best served, by far, by spending the small amount of money for an HSMAdvisor license. It will pay for itself many times over in shorter machining times, longer tool life, and fewer broken tools. You'll waste a huge amount of time and effort trying to do it yourself.

Regards,
Ray L.

[tmarks11]

....I deliberately measured the thickness of several of the Metal Shavings that flew off of my metal stock. Out of curiosity, I wanted to see if they were actually .015" thick...From these measurements I deduced that perhaps I needed to reduce the WOC

Like Ray said, WOC does not equal Chip Load (sometimes called Chip Load Per Tooth or Feed Per Tooth).

Chip Load = feed rate ( ipm )/( cutting rpm x number of cutting edges) --Note: usually this equation is solved to calculate feed rate based upon RPM and CL.

The tooling manufacturer generally recommends a CL based upon material and cutter diameter. This CL is chosen to maximize insert life, and prevent tool flexing/breaking. For example, in aluminum, a 0.5" endmill generally gets a recommended 0.004" CL, and a 1" endmill gets 0.007".

NOTE: If WOC when edge milling is actually driving CL size, then that means your feed rate is way more than is recommended by the tooling manufacturers.

Here are some good examples
Harvey Tool - Speeds and Feeds Guide | General Machining Guidelines
Niagara Cutter Speed and Feeds

in review:
1. select rpm based upon sfm and tool diameter.
2. select feed rate based upon rpm, CL, material, and diameter.
3. WOC/DOC based upon spindle hp available (this is the calculation where HSM Advisor or G_wizard helps out, the previous two are child's play).

If your chips are too blue or your spindle is bogging down, don't reduce your feed rate. That will make smaller chips, which means your cutter will heat up more and die faster. Instead adjust DOC or WOC so less power is required.

[SCzEngrgGroup]

Like Ray said, WOC does not equal Chip Load (sometimes called Chip Load Per Tooth or Feed Per Tooth).

Chip Load = feed rate ( ipm )/( cutting rpm x number of cutting edges) --Note: usually this equation is solved to calculate feed rate based upon RPM and CL.

And that equation works only for relatively wide cuts, where chip thinning does not come into play. For cuts with a small WOC, the chip will be MUCH thinner than that equation will calculate, which is why you can feed as much as 10X faster when taking a very narrow cut.

Regards,
Ray L.

[MetalShavings]

I'll give it another shot after I've sold off the batch of small parts I made up using conventional milling techniques. With Christmas coming up I'm hoping that alot of air rifles are under the Christmas trees this year. This will assure the sale of my present stock of specialty parts.

The parts in question are closer in shape to the Fish-Shaped parts I posted a zip file on. That's a whole new set of numbers as far as HSM tool paths are concerned. I think someone posted a set of numbers using a three-flute 3/8" coated carbide bit I can try.

I'll let you all know how it works out once I've tried it.

Thanks everyone.

MetalShavings