DIAbide Inserts

for Machining Non-Metallic Materials

and Non-ferrous Metals

Machining Guidelines

General Guidelines

Abrasion is the primary mode of tool wear with high silicon aluminum (10% silicon) and 390 aluminum (18% silicon), and with metal matrix composite materials such as DURALCAN® (20% silicon carbide). As the cutting edge of the tool encounters the hard particles in the aluminum matrix, these particles chip away tiny flakes of the tool edge, be it carbide or diamond. The greater the amount of workpiece material swept out by the tool, i.e. the deeper and/or wider the cut, the less the tool is abraded and the longer its life for a given amount of material removed.

Compared with a typical aluminum feed rate of 0.005 inch per revolution (ipr), with low silicon aluminum alloys, heavy roughing feed rates—in the order of 0.015 ipr—not only increase the material removal rate but also remove up to five times the volume of material per unit of tool wear. The volume removed equals the product of depth-of-cut, feed rate, cutting speed, and time. Tool life typically will be extended when the cutting speed is limited to 2000 surface feet per minute (sfm) or less.

If surface finish is an issue, sp³ recommends roughing at the maximum practical feed rate and depth-of-cut, followed by a single finishing pass at a lower feed rate and depth-of-cut. In automatic turning centers, install two DIAbide inserts—a general purpose insert and a finishing insert.

Depth of cut

The depth-of-cut should never exceed half the insert's leg length, and the feed should not exceed half of the nose radius. These precautions will reduce the likelihood of fracture of the cutting edge and of poor surface finish on the workpiece. The rake and clearance angles for machining abrasive materials will generally be the same as for unreinforced aluminum alloys. Select an insert with I.C. (Inscribed Circle) size according to the maximum depth-of-cut to be taken.

Cutting Speed

The graph shows how tool wear progresses fairly gradually with cutting speed until the "knee" in the curve is reached, at which point wear increases rapidly with increased cutting speed. If you experience short tool life, reduce the cutting speed until improved tool life shows you are working in the normal-life portion of the wear curve.

Feed rate

With sp³ DIAbide inserts, aggressive feed rates will remove more material (at the expense of surface finish) without materially accelerating tool wear and shortening tool life. In other words, tool life—in terms of cutting time—is largely independent of feed rate.

Coolant

Because of the lubricity of diamond, coolant isn't normally required when using DIAbide inserts. The ability to cut dry avoids contamination of the workpiece by the coolant.

A coolant (such as 5% water-soluble oil) may sometimes be used to improve surface finish and/or to enhance chip clearing. If you experience a built-up edge, try using a coolant. Using a coolant has little effect on tool life. If tool life does not meet expectations, reduce the cutting speed.

Select the smallest insert that will support the intended depth-of-cut.
The maximum depth-of-cut is half the cutting edge length.

Recommended Starting Parameters
Workpiece Material		Application	Turning, Facing and Boring		Milling
Workpiece Material		Application	Cutting Speed sfm	Feed Rate fpr (in/rev)	Cutting Speed sfm	Feed Rate fpt (in/tooth)
Non- ferrous metals	Free machining aluminum alloys (less than 12% silicon)	Rough Finish	2000 – 3000 3000 – 3500	.010 – .020 .003 – .010	2000 – 4000 2000 – 4000	.005 – .012 .003 – .008
	High (>12%) silicon aluminum alloys, aluminum matrix composites.	All*	1000 – 2500	.005 – .015	2000 – 4000	.005 – .012
	Free machining copper alloys, brasses, bronzes, lead, zinc	Rough Finish	1000 – 1500 1500 – 2000	.010 – .020 .003 – .010	500 – 1500	.002 – .006

Non- metallic materials	Unfilled plastics, graphite, carbon	Rough Finish	2000 – 3000 3000 – 4000	.010 – .020 .003 – .010	2000 – 4000	.003 – .008
	Reinforced plastics, composite materials	Rough Finish	500 – 1000 1000 – 1500	.008 – .020 .003 – .010	2000 – 4000	.003 – .010
	Green ceramics	All	100 – 500	.002 – .010	500 – 1000	.002 – .006
*General purpose where cosmetic finish is not critical. sfm = surface feet per minute. fpr = feed per revolution. fpt = feed per tooth per revolution.

For assistance call 888-547-4156

OverviewInsert CatalogApplications