Webinars

PI shapes cut easily with most circular, chop, or band saws. Follow these suggested guidelines for best results.

Table, Chop, or Panel Sawing:

• A 10"-16" diameter modified triple chip saw blade with 60 or 80 teeth and 0 degree to 5 degree positive rake operating at surface speeds ranging from 6,000 to 9,000 feet per minute will provide maximum results.
• A good vacuum system to remove dust and chips may improve results.
• In rare cases when chipping occurs, the saw blade may be too sharp and must be slightly dulled for better performance.

Band Sawing:

• Parts ranging from 1/8" to 5" thick can be easily cut with 6 to 10 vary tooth bi-metal construction blades.
• Feed and speeds vary from thickness of material.

Drilling, Reaming, Boring & Tapping:

The high strength and stiffness properties and insulating characteristics of PI require consideration during drilling operations to avoid seizing and chipping.

Drilling:

• Solid carbide twist drills with a 20 degree helix and a 118 degree included point angle provide the best chip removal.
• To maintain minimal heat build up, use a cold airgun or water-soluble coolant for maximum chip removal. This will increase surface finish and increase greater achievable tolerances.
• To avoid chipping or cracking around the hole, always use a backing plate when drilling a thru-hole. Recommended spindle speeds are between 3,000 to 4,000 RPM and feeds are between 10 to 40 IPM.
• For smaller holes in high production, solid carbide circuit board drills may provide better results.
• For larger holes, spot dripping and/or a pilot hole is recommended. Avoid hand feeding because of the drill grabbing, which can result in micro-cracks.

Reaming & Boring:

• When reaming or boring, a major consideration is temperature build-up. Use air or soluble coolants to eliminate any heat.
• Only use solid carbide or carbide-tipped tooling.
• When reaming thru-holes, the use of solid carbide high precision spiral reamers pushes the chips ahead of the finished hole, leaving a precisely reamed hole with excellent surface finish. This is also advantageous because the coolant is led straight to the cutting edge, preventing it from over heating while lubricating the reamed hole.
• Reamed holes should be drilled .003" to .005" undersized, with spindle speeds increased and feed rates decreased.
• Boring is preferred for close tolerance situations. leave the hole at least .005" to .010" undersized before boring.

Threading & Tapping:

• Threading should be performed with a carbide single-point insert. The depth of feed should not exceed .005" on the first pass, and gradual reduction to .001" per pass on the final five cuts, along with two spring passes, will ensure good thread quality.
• For optimum results when tapping, use the corresponding drill size with a two-flute carbide tap. Keep the tap free of chip build-up. The use of coolants and/or wax is also recommended.
• Countersink or produce a lead before threading or tapping. This will reduce chipping or cracking.
• In certain instances, drilling slightly oversize will produce a better thread.

Milling: (Vertical & Horizontal Machining)

• A good start to any successfully machined part begins with proper work holding. Be sure your work piece is properly held to ensure no vibration, thus giving you the surface finish you desire.
• XP-141T responds quite well to the following tooling:
• Carbide insertable fly cutters
• Two-flute solid micro-grain tungsten carbide end mills with 30- or 40- degree helix geometry
• C-2 grades of carbide end mills
• O-f1ute end mills
• In limited circumstances, cobalt and HSS tooling.
• For maximum machining speeds, carbide grades with a TiN (titanium nitride) or TiCN (titanium carbonitride) coating will produce less heat for longer cutter life.
• Many of the same milling operations employed on metal may be used on PI shapes, except that much higher spindle speed must be used.
• Some helpful hints when machining PI:
• Avoid heat build-up; use either air or soluble coolants
• Use rough and finish cuts when possible
• Slow your cross feeds when breaking through an edge, and save your profiling operation until last
• Use 4,000 to 6,000 spindle RPM and 10 to 30 IPM
• Employ conventional or climb milling for superior surface finish

Turning:

• Like milling, successful turning begins with the proper selection of work holding. The part dynamics will determine whether you employ a three-jaw or six-jaw chuck, 0D collet, 1D expansion collet, or custom machinable pie jaws. In all instances, distribute equal pressure throughout for zero distortion.
• Tooling techniques begin with carbide facing, boring, and turning inserts. For best results, use a high positive, 20 degree clearance angle with a .003" to .008" nose radius.
• Spindle speeds range from 3,000 to 5,000 RPMs. Rough cuts range from .010" to .010" IPR, while finish cuts range from .002" to .005" IPR.
• Avoid heat build-up through the use of air or soluble coolants.
• Most carbide grades of tooling used in milling operations translate well for turning operations.

Work Holding:

The main precaution in holding PI shapes for machining is distortion through over tightening, which may cause part deformation. Deflection can be prevented through proper chuck, vise, or fixture selection.