Tips for no-melt machining

Jack Sharp
Tooling & Fabrication Center
Manager
DSM Engineering Plastic Products
Reading, Pa.

EDITED BY JEAN M. HOFFMAN

Semiconductor-equipment manufacturers machine advanced plastic stock shapes such as this fully imidized thermoset polyimide (PI) into wafer clamp rings. With a continuous use temperature of 500°F along with high strength, stiffness, and chemical inertness the machinable PI helps ensure that the rings stand up to the ravages of wafer processing. Called Duratron XP, the material is a ductile PI and, as such, resists chipping, breakage, and tool wear during machining.

Surgical probes machined from Ultem PEI rod are autoclavable. PEI offers high strength, rigidity, and dimensional stability. However, because it is an amorphous material, nonaromatic coolants should be used when machined.

Aircraft engine electrical connectors machined from PBI plate are strong, dimensionally stable and can withstand temperatures over 400°F. Polycrystalline diamond tools are recommended when machining the PBI called Celazole, because it is an extremely hard material

Process and test equipment manifolds machined from a PET bar stock called Ertalyte PET-P offer good dimensional stability, combined with excellent stain and chemical resistance. Machined PET-P shapes have low residual stress and are porosity-free. Coolants are not required, but generally improve surface finishes and tolerances.

Makers of semiconductormanufacturing equipment have long been known as major users of plastics that work at high temperatures and that resist corrosion. What is interesting is that these materials serve in applications where conventional plastic-forming techniques either cost too much or won't allow quick and frequent design changes.

Take the example of a clamp ring for polishing silicon wafers. Frequent dimensional changes cropped up during design that made large-scale injection molding impractical. The cost of repeated tool rework would have been quite high. In contrast, the only cost associated with shaving a few thousandths off one of the clamp ring's features was in material and reprogramming.

Machinable plastic stock shapes span a wide performance and price range. They can significantly reduce weight, eliminate corrosion, reduce noise, and act as thermal and electrical insulators. New grades of advanced plastics are capable of long term service up to 800°F and even short stints at 1,000°F. Such qualities let designers put plastics where they never thought to put them before. New uses include bearings and wear surfaces as well as in static or dynamic structural applications.

Machinable, advanced plastic, stock shapes are made from a wide variety of imidized and crystalline polymers. They fill a niche for small to medium-quantity production runs or for parts needing tolerances tighter than is practical from conventional plastic-forming processes.

BEATING THE HEAT
Thermoplastic stock shapes are relatively easy to machine. But they do not necessarily respond like metal plate, rod, and bar when drilled, turned, or milled. One reason is that their thermal expansion is up to 10 times larger than that of metal. During drilling, for example, thermoplastics can heat up and expand, then cool off and contract. The resulting hole will most likely be undersized.

Another reason that plastics don't machine like metal is their low thermal conductivity. This makes it difficult to cool them during machining. They will soften, deform, or even melt if the heat generated is not effectively removed.

Common ways to reduce heat include removing less material or extending the machining time with slower feed rates. Another is peck drilling — alternating between drilling and retraction or pull-out from the work piece.

A two-step, drilling/boring process works well for notch-sensitive materials. These include poly-ethylene terephthalate (PET), polyamide-imides (PAI), polyimides (PI), and polybenzimidazole (PBI), as well as their carbon and glass fiber-reinforced counterparts. The two-step process minimizes heat buildup and reduces the risk of cracking.

For general sawing operations, good blade design can reduce the frictional heat between tool and part. For example, the angle formed between the tooth face and a line passing through the blade's rotational axis or rake angle should be 0° for rip and combination blades. The teeth should also be offset from the blade centerline by 3 to 10°.

Coolants, are not typically necessary for many thermoplastic machining operations. They are essential, however, for drilling and parting. But, common cutting fluids for metals are solvents that tend to attack plastics and accelerate stress crazing or cracking during machining. The best coolants for plastics include high-pressure air, water, and nonaromatic, water-soluble cutting fluids. Keeping the cutting area cool generally helps improve surface finish and tolerances. The use of a coolant is essential when drilling notch-sensitive materials.

It's also important to look at the wide array of profiles available when selecting stock shapes. Stock shapes are made by compression and injection molding, extrusions, and castings. The process used to make the stock shape often has little bearing on the choice of material. But the initial forming technique can indeed affect some physical properties. For example, injection-molded shapes show the greatest directionally dependent or anisotropic behavior. Extruded shapes are slightly anisotropic. Compression molded shapes, on the other hand, are isotropic. They show equal properties in all directions.

MACHINING TIPS
Guidelines for machining thermoplastic stock shapes take into consideration their notch sensitivity and lower strength compared to metals.

Among the first considerations is adequate support for the plastic during machining. This helps keep the plastic from deflecting away from the cutting tool or cracking when the tool breaks the surface.

Chip-flow management is also important. The use of positive air pressure directs or removes chips from the work area. This is important because errant chips are prone to either interfere with the cutter or heat up and melt onto the workpiece. The use of suction nozzles and collection systems readily deposits milled chips into containers for easy cleanup.

Cutting tools should have positive geometries and ground peripheries. Carbide tooling with polished top surfaces generally last the longest and give good surface finishes. For finish cuts, stay away from insert tools with molded edges.

Turning operations require inserts such as fine-grained C-2 carbide. Generally, polished top surfaces and ground peripheries reduce material buildup on the insert. This, in turn, improves the surface finish. Diamond-coated and polycrystalline tooling are said to provide the best surface finishes when machining PI or PBI which are harder and notch sensitive.

Drilling requires special considerations because of the thermal insulating nature of plastics, particularly when hole depths exceed twice the diameter. High-speed steel M10, M7, or M1 bits work well with the various engineering resins.

For small-diameter holes of <1 in., high-speed steel twist drills generally are sufficient. Peck-drilling and the use of a slow-spiral, low helix drill improves chip or swarf removal as well as helping eliminate heat. For large diameter holes of >1 in., a slow-spiral, low helix or general-purpose drill bit ground to a 118° point angle with 9 to 15° lip clearance is recommended. In addition these bits should have their lip rake ground or dubbed off and their web thinned.

Generally, it's best to drill pilot holes of up to 0.5-in. diameter at rates from 600 to 1,000 rpm with positive feeds of 0.005 to 0.015 in./rev. Avoid hand feeding because drill grabbing causes microcracks. To expand the hole diameter further, use secondary drilling rates of 400 to 500 rpm at 0.008 to 0.020 in./rev. Threading should take place using a single point tool with a carbide insert. Keep the workpiece cool and take four to five 1-mil passes at the end. For tapping, cool the work piece and use the specified drill with a two-flute tap. It's also important to keep the tap clean of chip buildup.

End Milling, the most versatile milling operation, is used for slotting, contouring, and making cavities among others. Good holding fixtures are a must to end mill plastics at high spindle speeds and fast table travel.

Face milling tools square the end of a piece of stock and give it a smooth finish. They should either have high-positive or high-shear geometry cutter bodies. C-2 carbide tools with positive geometry cutter bodies are the most standard type.

Sawing also falls under the auspices of machining. Band sawing is versatile for straight, continuous curves or irregular cuts. Table saws are also convenient for straight cuts. With adequate horsepower, table saws easily cut multiple thicknesses and cross sections up to four inches. Saw blade selection is generally based on material thickness and desired surface finish. Tungsten carbide blades resist wear and provide good surface finish. Hollow ground circular saw blades without set yield smooth cuts up to 0.75 in.

ANNEALING
Any operation that removes material or creates heat generally causes internal stresses in thermoplastics. This includes machining operations such as drilling, turning, and milling. Machinedin stress reduces part performance and often leads to premature part failure. A number of different factors can create these stresses. Dull or improperly designed tooling is one. Another may be the excessive heat generated from inappropriate speeds and feedrates. Stresses may result if the stock shape has large volumes of material machined from only one of its sides.

The best way to reduce machined-in stress is to follow the fabrication guidelines presented for each specific material. Extremely close-tolerance parts having precision flatness or nonsymmetrical contours need intermediate annealing steps between the various machining operations. For example, improved flatness often comes from a rough machining step followed by annealing, then light cutting to remove only a small volume of material during final finishing.

Furthermore, postmachining annealing often improves chemical stress-crazing resistance for transparent amorphous plastics such as polycarbonate (PC), polysulfone (PSU), and polyetherimide (PEI). Similarly, it also boosts the wear resistance of PAI parts.

DESIGN SUGGESTIONS Here are some quick and dirty rules of thumb for machined engineered thermoplastics: Inside corner radius should range from 0.015 to 0.030 in. Outside corners should have round edges with minimum radii of 0.005 in. or 0.005-in. minimum chamfers. Adjacent holes drilled near an outside surface need at least one full diameter distance between them. Press fits into straight-sided holes are preferred, especially on internally pressurized parts, rather than drilled and tapped fittings. Threaded fasteners need some clearance at the bottom of a drilled/tapped hole. Tolerances typically run about ± 0.1 to 0.2% of the machined dimension. Surface finishes on the order of 30 to 60 RMS are common, but depend on tooling and machining techniques employed.

TROUBLESHOOTING TIPS: DRILLING: Tapered holes often come from incorrectly sharpened drills, insufficient clearance, and feedrates that are too heavy. Melted or burned surfaces commonly result from the wrong type of drill, one that is incorrectly sharpened, or even one that's dull. Feed that's too light also generates burned surfaces. Chipped surfaces arise with heavy feed or when there's too much clearance or rake angle. Chatter comes from too much clearance or rake as well as light feed. It also turns up if the drill overhang is too great. Feed marks on inside diameters are a consequence of a noncentered drill or one that's been ground off center. The marks or spiral lines also are generated if the feed's too heavy. Oversized holes are a result of drills ground off-center or those with small points or thick webs. They also happen when there's insufficient clearance and heavy feed. Undersized holes, on the other hand, come from too much clearance and dull drills. In addition, a small drill point may also reduce the intended hole size. Nonconcentric holes come from many sources. Among the culprits are drills not mounted on center or sharpened correctly. Drills with thick webs or those started too heavy or driven into the underlying workpiece will distort the drilled hole. Other sources to look for include nibs left by cut-off tools which sometimes deflect the tool as it's drilling, or spindle speeds that are too slow. CUTTING OFF OR PARTING: Melted surfaces crop up if there's insufficient side clearance or not enough coolant supply. A dull tool may also heat the plastic to its melting point. Rough surfaces turn up when a tool is improperly sharpened or its cutting edge is not honed. Additionally, heavy feed also tends to roughen plastics. Spiral marks appear if the tool rubs during its retreat or if there's a burr on its point. Concave or convex surfaces arise when tools are mounted above or below center or are not perpendicular to the spindle. In addition, heavy feed or tool deflection also brings about hills and valleys in the workpiece. One method of thwarting tool deflection is the use of a negative rake. Nibs or burrs at cut-off point come when the tool's dull, when its point angle is too small, or when its feed is too heavy. TURNING AND BORING: Melted surfaces tend to be associated with dull tools, insufficient side clearance, slow feed rates, and spindle speeds that are too fast. Burrs at edge of cut also come from dull tools and insufficient clearance angle as well as a lack of a lead angle — the tool should ease out of a cut gradually, not suddenly. Rough finishes come from heavy feeds, incorrect clearance angles, and tools not mounted on center. Sharp pointed tools often contribute to rough finishes, so it's recommended that tools have a slight nose radius. Cracked and chipped corners happen when there's too much positive rake on the tool, when it's dull or mounted below center. Cracks and chips also propagate when the tool isn't eased out of the cut gradually or if it has a sharp point. Chatter often stems from tools with too much nose radius or those not solidly mounted. It also happens when the material is not supported prop-erly or if the cuts are too wide.

Machining parameters for turnings
MATERIALS	DEPTH OF CUT, in.	SPEED, fpm	FEED, in./rev
POM, PA, PEEK,	0.025	600 to 700	0.004 to 0.007
PC, PEI, PET, PSU	0.15	500 to 600	0.01 to 0.015
PAI	0.025	300 to 800	0.004 to 0.025
PBI, PI	0.025	150 to 225	0.002 to 0.006
	0.15	100 to 150	0.005 to 0.01
PPS	0.025	250 to 500	0.005 to 0.01
	0.15	100 to 300	0.01 to 0.02

Typical properties of engineering materials
BASE RESIN	ABBREVIATION	DENSITY (gm/cm 3)	TENSILE STRENGTH (ksi)	MODULUS OF ELASTICITY (ksi)	COEFFICIENT OF LINEAR THERMAL EXPANSION ( in./in./ °F)
Nylon	PA	1.15	12	450	50
Polyamide-imide	PAI	1.45	18	600	14
Polybenzimidazole	PBI	1.3	23	836	13
Polycarbonate	PC	1.2	10.5	319	39
Polyetheretherketone	PEEK	1.31	16	500	26
Polyetherimide	PEI	1.28	17	475	31
Polyethylene terephthalate	PET	1.41	12.4	460	33
Polyimide	PI	1.41	18	600	17
Acetal	POM	1.33	5.4	200	90
Polyphenylenesulfide	PPS	1.55	10	800	12
Polysulfone	PSU	1.24	10	360	31
Steel (A36)	—	7.84	36	30,000	6.3
Aluminum	—	2.7	30	10,000	12

Drilling guidelines
MATERIALS	NOMINAL HOLE DIAMETER, in.	FEED, in./rev
POM, PA, PPS,	0.0625 to 0.25	0.007 to 0.015
PSU, PEI, PET,	0.5 to 0.75	0.015 to 0.025
PC, and PAI	> 1	0.02 to 0.05
PBI, PI	0.0625 to 0.25	0.005 to 0.0015
	> 0.5	0.015 to 0.025
PEEK	0.0625 to 0.250	0.002 to 0.005
	0.5 to 0.75	0.004 to 0.008
	> 1	0.008 to 0.012
PPS	0.0625 to 0.25	0.007 to 0.015
	0.5 to 0.75	0.015 to 0.025
	> 1	0.02 to 0.05

Helpful advice on end milling
MATERIALS	DRILL BIT SIZE	DEPTH, in.	SPEED, fpm	FEED, in./tooth
POM, PA,	0.25	0.25	270 to 450	0.002
PC, PAI,	0.5	0.25	270 to 450	0.003
PEEK, PEI,	0.75	0.25	270 to 450	0.005
PET, and PSU	1 to 2	0.25	270 to 450	0.008
	0.25	0.05	300 to 500	0.001
	0.5	0.05	300 to 500	0.002
	0.75	0.05	300 to 500	0.004
PPS	0.25	0.25	270 to 450	0.002
	0.5	0.25	270 to 450	0.003
	0.75	0.25	270 to 450	0.005
	1 to 2	0.25	270 to 450	0.008
	0.25	0.05	300 to 500	0.001 to 0.002
	0.5	0.05	300 to 500	0.003 to 0.005
	0.75	0.05	300 to 500	0.005 to 0.01
PBI and PI	0.25	0.05	270 to 450	0.002
	0.5	0.05	270 to 450	0.003
	0.75	0.05	270 to 450	0.005
	1 to 2	0.05	270 to 450	0.008
	0.25	0.015	300 to 500	0.001
	0.5	0.015	300 to 500	0.002
	0.75	0.015	300 to 500	0.004

Face milling guidance
MATERIALS	DEPTH OF CUT, in.	SPEED, fpm	FEED, in./tooth
POM, PA, PC, PEI,	0.15	1,300 to 1,500	0.02
PET, PPS, and PSU	0.06	1,500 to 2,000	0.005
PAI	0.035	500 to 800	0.006 to 0.035
PBI and PI	0.05	450 to 650	0.005 to 0.01
	0.015	250 to 350	0.002 to 0.006
PEEK	0.15	500 to 750	0.01
	0.06	500 to 750	0.005

Sawing primer
MATERIALS	MATERIAL THICKNESS, in.	TOOTH FORM	PITCH teeth/in.	BAND SPEED, fpm
POM and PA	<0.5	Precision	10 to 14	3,000
	0.5 to 1	Precision	6	2,500
	1 to 3	Buttress	3	2,000
	> 3	Buttress	3	1,500
PC	<0.5	Precision	10 to 14	4,000
	0.5 to 1	Precision	6	3,500
	1 to 3	Buttress	3	3,000
	> 3	Buttress		2,500
PAI and PET	<0.5	Precision	10 to 14	5,000
	0.5 to 1	Precision	6	4,300
	1 to 3	Buttress	3	3,500
	> 3	Buttress	3	3,000
PEEK, PEI,	<0.5	Precision	8 to 14	4,000
and PSU	0.5 to 1	Precision	6 to 8	3,500
	1 to 3	Buttress	3	3,000
	> 3	Buttress	3	2,500
PPS	<0.5	Precision	8 to 14	5,000
	0.5 to 1	Precision	6 to 8	4,300
	1 to 3	Buttress	3	3,500
	> 3	Buttress	3	3,000
PBI and PI	0.375 to 1	Precision	10	3,000
	1 to 2	Buttress	10	1,500

Post machining annealing
MATERIALS	HEAT UP (°F)	HOLD	COOL DOWN (°F/h)	ENVIRONMENT
PA and PET	4 h @ 350	30 min/0.25 in.	50	Oil or nitrogen
POM	4 h @ 310	30 min/0.25 in.	50	Nitrogen or air
PC	4 h @ 275	30 min/0.25 in.	50	Air
PSU	4 h @ 330	30 min/0.25 in.	50	Air
PEI	4 h @ 390	30 min/0.25 in.	50	Air
PES	4 h @ 390	30 min/0.25 in.	50	Nitrogen or air
PPS	4 h @ 350	30 min/0.25 in.	50	Air
PEEK	2 h @ 300 or 375	60 min/0.25 in.	50	Air
PAI	4 h @ 300, 420, 470	24 h	50	Air
	or 4 h @ 500	3 to 10 days	50	Air