General Fabrication Guidelines

The following guidelines are presented for those machinists not familiar with the machining characteristics of plastics. They are intended as guidelines only, and may not represent the most optimum conditions for all parts. The troubleshooting quick reference in this section should be used to correct undesirable surface finishes or material responses during machining operations.

Most quality stock shape materials are stress relieved to ensure the highest degree of machinability and dimensional stability. However, the relative softness of plastics (compared to metals) generally results in greater difficulty maintaining tight tolerances during and after machining. A good rule of thumb for tolerances of plastic parts is +/- .001 per inch of dimension although tighter tolerances are possible with very stable, reinforced materials.

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 polished top surfaces is suggested for optimum tool life and surface finish. Diamond coated or polycrystalline tooling provides optimum surface finish when machining Duratron® XP or Vespel®
PI or Celazole* PBI.

Use adequate chip clearance to prevent clogging
Adequately support the material to restrict deflection away from the cutting tool
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.

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

Band sawing is versatile for straight, continuous curves or irregular cuts. Table saws are convenient for straight cuts and can be used to cut multiple thicknesses and thicker cross sections up to 4” with adequate horsepower. Saw blades should be selected based upon material thickness and surface finish desired.

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

Small diameter holes (232″ or 1mm to 1.0 or 25mm)
High speed steel twist drills are generally sufficient for small holes. To improve swarf removal, frequent pull-out (peck drilling) is suggested. A slow spiral (low helix drill will allow for better swarf removal.

Large diameter holes (1.0” or 25mm 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, Torlon* PAI, Duratron® XP, Vespel® PI, Celazole* PBI and glass or carbon reinforced products. This minimizes heat build-up and reduces the risk of cracking.

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.
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.
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.

Coolant Recommendations

Coolants are generally not required for most plastic 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 metals and some plastics, may contribute to stress cracking of amorphous plastics such as Acrylic, Polycarbonate, Polysulfone, Ultem® PEI, and Radel® R PPSU.

Coolants Tips
Coolants are strongly suggested during drilling operations, especially with notch sensitive materials such as Ertalyte® PET-P, Torlon® PAI, Duratron® XP, Vespel® PI, Celazole® PBI and glass or carbon reinforced products.
In addition to minimizing localized part heat- up, coolants prolong tool life. Example (flood) coolants suitable for most plastics include:
Cimstar 40B (CimCool Milacron, Cincinnati, OH)
Trim 9106CS (Master Chemical, Perrysburg, OH)
Polycut (Tullco, Savannah, GA).
A generally suitable mist coolant is Astro-Mist 2001A (Monroe Fluid Technology, Hilton, NY).

Machining Tips

Rip and combination blades with a 0° tooth rake and 3° to 10° tooth set are best for general sawing in order to reduce frictional heat.
Hollow ground circular saw blades without set will yield smooth cuts up to 3/4” thickness.
Tungsten carbide blades wear well and provide optimize surface finishes.