Jason:
I retired from Kennametal 3 years ago after 35 years of service. Since retirement, Kennametal purchased Stellram, so I don't know much about their offering under the Kennametal umbrella. However, Stellram makes some really good milling products and some really excellent small parts tools for turning and other standard stuff as well. The design in the ad is considered a "high feed" mill due to the low, approximately 15 deg. approach angle. Stellram high feed cutter inserts have a curved edge as is noted by the "X" (wild card-anything goes) in the first position on the insert package. But for explanation we will call it a 15 deg. angle. These tools produce high axial force into the spindle and low radial force. This means that you would be producing an equal amount of downward force on the part. So, a not so stable part with a thin cross section would probably be somewhat unstable coming onto the part and leaving the part. Do not set your depth of cut to anything greater than the height of the 15 degree angle. Typical cutters of this type require high feed rates because of the extreme chip thinning that takes place with the low lead angle. Feed rates for typical zero degree lead cutters are .003 to .010 per tooth per rev., but your cutter is probably comfortable in the .015 to .040 chip load per tooth range. For example, a 45 degree lead cutter with a .010 chip load per tooth will produce a chip of only .707 (sine of 45 deg.) x .010, or .00707 thickness. .010 feed rate at a 15 degree lead would produce a chip thickness of only .0026. To achieve a .010 chip thickness the feed will have to be nearly .040 per tooth. These tools require high feeds to make the inserts function properly. An example for your tool would be to run, lets say .060 depth of cut, with half of the tool engaged on a low carbon steel. Lets use 3 inches as our cutter diameter and 1.5 inches as our radial width of cut. Metal removal rates (MRR) are expressed in cubic inches per minute and are easy to calculate. Cubic anything requires Length x Width, x Height. Your cutter has 5 teeth and we will use a feed rate per tooth of .025". Bottom end for low carbon steel would be around 400 SFM. 400SFM on a 3 inch cutter is 509 RPM. 509 x 5 teeth x .025 = 63.625 IPM feed rate. Length = 63.625,
Width =1.5, height =.060.
MRR= 63.625 x 1.5 x .060= 5.73 cubic inches per minute. Low carbon steel requires roughly .9 horsepower per cubic inch of metal removed. This example will require 5.73 ci x .9 = 5.16 horse power.
Ken, above, recommends TPG32 style inserts. Great advise, every manufacturer I know still makes TPGs. What to look for... Make sure there is a "G" in the third position. That indicates that the tool is ground to a +/-.001 tolerance and will typically have a sharp edge. Look for a grade that has high toughness. ONLY buy PVD coated or uncoated grades if you want to have a sharp edge. CVD coatings ALWAYS require a honing operation to keep coating build-up at the cutting edge to a minimum, typically .001 to .002 radius. On light duty machines, feed rates per tooth should be low. With honed inserts, using a feed of .001 to .002 simply produces rapid wear, high heat, potential work hardening, and significant burrs.
Also, all of these TPG inserts work great in a standard or make your type tool holder for turning, facing or boring.
Good Luck,
Make something neat this weekend!
Gary
