Machinists Toolkit

When machining plastic stock shapes, remember...

• Thermal expansion is up to 10 times greater with plastics than metals
• Plastics lose heat more slowly than metals, so avoid localized overheating
• Softening (and melting) temperatures of plastics are much lower than metals
• Plastics are much more elastic than metals

Because of these differences, you may wish to experiment with fixtures, tool materials, angles,speeds and feed rates to obtain optimum results.

Getting Started

• Positive tool geometries with ground peripheries are recommended
• Carbide tooling with ground top surfaces is suggested for optimum tool life and surface finish. Polycrystalline diamond tooling provides optimum surface finish when machining Duratron® PBI.
• Use adequate chip clearance to prevent clogging
• Adequately support the material to restrict deflection away from the cutting tool

Coolants
Coolants are generally not required for most machining operations (not including drilling and parting off). However, for optimum surface finishes and close tolerances, non-aromatic, water soluble coolants are suggested. Spray mists and pressurized air are very effective means of cooling the cutting interface. General purpose petroleum based cutting fluids, although suitable for many metals and plastics, may contribute to stress cracking of amorphous plastics such as  PC 1000,  PSU, Duratron® U1000 PEI, and PPSU.

Machining Tips

• Coolants are strongly suggested during drilling operations, especially with notch sensitive materials such as Ertalyte® PET-P, Duratron® PAI, Duratron® PBI and glass or carbon reinforced products.
• In addition to minimizing localized part heat-up, coolants prolong tool life. Two (flood) coolants suitable for most plastics are Trim E190 and Tim Sol LC SF (Master Chemical Corporation-Perrysburg, OH).

Threading and Tapping

Threading should be done by single point using a carbide insert and taking four to five 0.001" passes at the end. Coolant usage is suggested. For tapping, use the specified drill with a two flute tap. Remember to keep the tap clean of chip build-up. Use of a coolant during tapping is also suggested.

Milling

Sufficient fixturing allows fast table travel and high spindle speeds when end milling plastics. When face milling, use positive geometry cutter bodies.

Milling Tips

Climb milling is recommended over conventional milling (see Diagrams).

End Milling / Slotting Guidelines

⁽¹⁾ For Fluorosint MT-01 PTFE contact Mitsubishi Chemical Advanced Materials' Technical Service team

Face Milling
(C-2, Carbide Tool)
 

⁽¹⁾ For Fluorosint MT-01 PTFE contact Mitsubishi Chemical Advanced Materials' Technical Service team

Drilling

The insulating characteristics of plastics require consideration during drilling operations, especially when hole depths are greater than twice the diameter.

Small diameter holes
(1/32" to 1" diameter)

High speed steel twist drills are generally sufficient for small holes. To improve swarf removal, frequent pullout (peck drilling) is suggested. A slow spiral (low helix) drill will allow for better swarf removal.

Large diameter holes
(1" diameter and larger)

A slow spiral (low helix) drill or general purpose drill bit ground to a 118° point angle with 9° to 15° lip clearance is recommended. The lip rake should be ground (dubbed off) and the web thinned.

It is generally best to drill a pilot hole (maximum 1/2" diameter) using 600 to 1,000 rpm and a positive feed of 0.005" to 0.015" per revolution. Avoid hand feeding because of the drill grabbing which can result in microcracks forming. Secondary drilling at 400 to 500 rpm at 0.008 to 0.020" per revolution is required to expand the hole to larger diameters.

A two step process using both drilling and boring can be used on notch sensitive materials such as Ertalyte® PET-P and glass reinforced materials. This minimizes heat build-up and reduces the risk of cracking.

1. Drill a 1" diameter hole using an insert drill at 500 to 800 rpm with a feed rate of 0.005" to 0.015" per revolution.

2. Bore the hole to final dimensions using a boring bar with carbide insert with 0.015" to 0.030" radii at 500 to 1,000 rpm and a feed rate of 0.005 to 0.010" per revolution.

⁽¹⁾ For Fluorosint MT-01 PTFE contact Mitsubishi Chemical Advanced Materials's Technical Service team

Turning

Turning operations require inserts with positive geometries and ground peripheries. Ground peripheries and polished top surfaces generally reduce material build-up on the insert, improving the attainable surface finish. A fine grained C-2 carbide is generally best for turning operations.

Turning Tips

Inserts with positive geometries and ground peripheries.

• Use recommended Turning Tooling Geometry (see Diagrams).

Turning Guidelines
(C-2, Carbide Tool)

⁽¹⁾ For Fluorosint MT-01 PTFE contact Mitsubishi Chemical Advanced Materials's Technical Service team

Annealing

When should parts be annealed after machining to ensure optimum part performance?

Experience has shown us that very few machined plastic parts require annealing after machining to meet dimensional or performance requirements.

All Mitsubishi Chemical Advanced Materials stock shapes are annealed using a proprietary stress relieving cycle to minimize any internal stresses that may result from the manufacturing process. This assures you that the material will remain dimensionally stable during and after machining.

Machined-in stress can reduce part performance and lead to premature part failure. To prevent machined-in stress, it is important to identify the causes.

Machined-in stress is created by:

• Using dull or improperly designed tooling
• Excessive heat - generated from inappropriate speeds and feed rates
• Machining away large volumes of material -usually from one side of the stock shape

To reduce the potential for machined-in stress, review the fabrication guidelines for the specific material. Recognize that guidelines change as the material type changes.

Post Maching
Benefits of Post-Machining Annealing

Improved Chemical Resistance
Polycarbonate, polysulfone, and Ultem® PEI, like many amorphous (transparent) plastics may be annealed to minimize stress crazing. Duratron® PAI also benefits from post machining annealing. Annealing finished parts becomes more important as machining volume increases. Annealing after machining reduces "machined-in" stresses that can contribute to premature failure.

Better Flatness and Tighter Tolerance Capability
Extremely close-tolerance parts requiring precision flatness and nonsymmetrical contour sometimes require intermediate annealing between machining operations. Improved flatness can be attained by rough machining, annealing and finish machining with a very light cut. Balanced machining on both sides of the shape centerline can also help prevent warpage.

Improved Wear Resistance
Extruded or injection molded Duratron® PAI parts that require high PV's or the lowest possible wear factor benefit from an additional cure after machining. This curing process optimizes the wear properties. Only PAI benefits from such a cycle.

Annealing Tips

• Ensure parts are fixtured to desired shape or flatness.
• Do not unfixture until parts have completed entire cycle and are cool to the touch.
• Do not take short-cuts.

Finish machining of critical dimensions should be performed after annealing.

Important: Annealing cycles have been generalized to apply to a majority of machined parts. Changes in heat up and hold time may be possible if cross sections are thin. Parts should be fixtured during annealing to prevent distortion.

Climb milling is recommended over conventional milling (see Diagrams).

• Ensure parts are fixtured to desired shape or flatness.
• Do not unfixture until parts have completed entire cycle and are cool to the touch.
• Do not take short-cuts.