"Plastic is not metal" this will be the talk for today, the first lesson fabricators will discover when attempting to machine plastic for the first time. Plastics and metals both are technically "machine-able," those similarities will end there.
Many metals are typically pure materials, plastics are however a blend or hybrid of different compounds. Metals typically hold their shape and have predictable melting points; plastics can expand five (5) or more times their original dimension with different heat tolerances. Machining metals typically has a predictable pattern with minimal creep, plastic on the other hand require quick adjustments, accommodation to creep, melting during machining and chipping. As you see we are stating the simple or basic principles of machining metals do not apply to machining plastics.
With experience and some guidance, the right material selection, proven handling techniques, proper tools and coolants, machining plastic components is attainable and achievable.
The goal of this insight blog is to technically demystify machining plastics. We will explore some of plastic's properties, expansion rates, tolerances, price, selection criteria and discussions on tool selection for some machining techniques. Fully understanding the differences between machining plastics over machining metals, will improve your designs and the quality and/or performance of your next components.
Material Selection of Cost vs. Performance: How should we go about selecting the ideal material for an application? Plastics outperform "traditional" metals, yet there is still widespread belief that this is not true. Bronze, stainless steel, and cast iron have been replaced by plastics with excellent results, plastics excel in high temperature and extreme working environments. Let's move to cost over performance, plastics are not cheap, and some high-performance formulas are more expensive than metal. A Polybenzimidazole (PBI-Celazole) is 25 times higher than cold rolled steel or 15 times the cost of Type 303 stainless steel. At these prices it is critical to employ the right machining techniques to reduce scrap of these costly engineered materials.
We feel the decision of a material type should be the investment in performance over cost. A higher quality material will yield a higher quality component, and can save you from in-field failures that lead to costly recalls in the future. In our experience it is better to invest up-front and in the beginning to avoid these hazards or setbacks...
What drives the choice for plastic over metal materials? Ponder the advantages of plastic
machined components with these few listed abilities to:
1. Eliminate Corrosion
2. Extend Service Life
3. Improve Wear Performance
4. Insulate/Isolate (Thermally and Electrically)
5. Lower Noise Level
6. Reduce Component Weight
Material Selection of Thermoplastic vs. Thermoset: Our first look into the material selection briefly touched on the costs associated with plastic materials, from that point a question then becomes " which category of plastics should be chosen?".
Thermoset plastic retains their solid state indefinitely and only have a few trade names,
thermoplastics on the other hand can be melted more than once to form new shapes.
Thermoplastics are the largest group of plastics and are the type best suited to be machined, the list below touches on some of the characteristics of these two (2) categories:
THERMOSET PLASTICS:
Are usually brittle and chip easily
Do not melt since chemically changed in molding
Often incorporate fillers as part of the composite
Common formulas:
1. Epoxy
2. Melamine
3. Micartas
4. Phenolic
5. PTFE
THERMOPLASTICS:
Melt and reform without changing chemically
Largest Class of Plastics
Diverse list of trade and generic names including:
1. Acetal
2. ABS
3. Nylon
4. Polyethylene
5. PVC
6. Teflon
Filler Options Include:
1. Carbon Fibers
2. Glass Fibers
3. Graphite
4. Carbon
5. Molybdenum Disulfide
6. PTFE
Note: It is important to talk about brand name recognition, in this industry brand name can lead to an automatic material order. Caution of this plastic material "Name Game" where each processor names "Their" own material for what is essentially a trade name material. Acetal is a generic material with several different market names for it, DuPont calls its version Delrin®, Hoechst calls it Hostform®, Celcon® calls it Celeanse, Quadrant calls certain Acetal versions Acetron®, and Ensinger-Hyde calls it Hydex®. Just these five (5) different names to brand one single material, this causes an unnecessary confusion in the marketplace.
There are many companion papers out there from plastic distributors on the hazards of unknowingly purchasing counterfeit materials, a good read is the common material is Rulon for bearing applications.
Conclusion: Cost is important, but materials should be selected based on their application, performance and "true trade names".
Machining vs. Injection Molding: After a proper plastic material has been selected, the next question to ask is "should this component be injection molded or machined?". The most cost-effective method for piece price is injection molding, most plastic products are produced this way. However it is best suited for high production, loose tolerances and other factors. Here is a list on what makes a better fit for machined plastic components:
1. Low Initial Costs - Machining is more economical for lower volumes and prototypes.
Quick part iterations or modifications during a production run. Injection molding
requires molding equipment and a large initial investment in tooling (Molds)..
2. Tight Tolerances - Machining can obtain much tighter dimensional tolerances than
achieved with injection molded parts.
3. Physical Property Limitations - There are materials such as PTFE and UHMW that
can't be injection molded and require to be machined from there raw state.
4. Stress Factors - Machined parts are more consistent due to the less internal stresses of
extruded rod, tube and sheet. Injection molded parts are produced under high pressures
there for creating more stress than extruded materials.
Some applications that use machined plastic components include : Semiconductor processing components, heavy equipment wear parts, and food processing components to name a few.
Let us move to the machining basics of working with plastics, this next section is from experiences and from tips and tricks gathered over the years from other contributors to this field of machining plastics. Please note these are suggestions and should be tried and experimented with at your own discretion. Do not machine actual final part sizes or production runs without first experimenting with tips on scrap materials of various plastic grades.
Machining Plastics 101: Keeping it Cool
With machining plastic materials the most important factor is to limit the build up of heat,
the very act of machining produces friction and generates heat. Keep in mind that anytime
you cut or machine plastic (especially dry) your cutting tool can instead become "a tool for
melting plastic". Heat also creates dimensional challenges do to the part expanding making
it difficult to hold tight tolerances, due to poor thermal conductivity and lower melting
properties the main skill is to avoid heat build up and evacuate swarf.
1. When machining Nylons, UHMW PE and softer materials go for maximum feed and
speed to get swarf away from the tool and avoid swarf build up or wrap around.
2. Select tools with large clearance to allow swarf evacuation and deeper cuts.
3. Use Milling cutters with 2 or three flutes with higher helix angles.
4. Try to use air blast (Meech Air Blasters) or vacuum venturi instead of a liquid coolant.
5. HSS works well but solid carbide is stiffer.
6. Glass or carbon filled plastics use carbide or PCD, reduce speed and increase feed rates.
1. Drilling Operations: Drilling generates the most heat than in any other operation.
Many plastics with a high expansion rate have low melt temperatures. UHMW has an expansion rate of 20 times that of steel and melts at 266°F, adding fillers brings another level to the expansion rate making it difficult to predict. PEEK (unfilled) expands twice as much as a 30% carbon filled PEEK material, and adding PTFE to PEEK raises the expansion rate slightly while none of these fillers changed the melt temperature. Getting back to drilling, plastics can build up heat very easily during drilling operations that are greater than twice the drill diameter.
1. Use twist drills with twist angles between 12 - 18 degrees. The large flute area assists in
chip evacuation.
2. Cutting edge should be ground with one edge being 0.005" to 0.010" longer than the
other.
3. Blunt angles of 115 to 130 degrees for thin-walled pieces to prevent the OD from
expanding.
4. Grind relief on to drills of 20 - 50 degrees will reduce friction, angles will vary based on
the material choice, but it is a good starting point and testing will be required.
5. With softer materials the use of high speed steel drills are adequate, if using highly
abrasive plastic (filled materials) requires the use of carbide (Titanium Nitrite/TiN/
AlTiN), CVD (chemical vapor deposition) diamond, or PCD (polycrystalline diamond)
tooling.
6. Higher frequency of "pecking" to remove chips and give the material a chance to cool
slightly is preferred. The deeper the hole the more the drill should be removed from the
hole.
7. Reduced RPMs can be beneficial depending on the material and other conditions of
coarse. Here is a list of reasonable starting points to try based on drill size:
A. No. 60 thru 33 ---- 5,000 rpm
B. No. 32 thru 17 ---- 3,000 rpm
C. No. 16 thru 01 ---- 2,500 rpm
D. 1/16" thru 7/64" -- 5,000 rpm
E. 1/8" thru 11/64" -- 3,000 rpm
F. 3/16" thru 15/64" - 2,500 rpm
G. 1/4" thru 5/16" --- 1,700 rpm
H. 3/8 thru 13/32" --- 1,300 rpm
I. 7/16" thru 1/2" ---- 1,000 rpm
J. A thru D ------------ 2,500 rpm
K. E thru M ----------- 1,700 rpm
L. N thru Z ------------ 1,300 rpm
8. Use new or drills that have never drilled metal, tool may be to dull and will impact
tolerances and/or surface finishes.
9. It is advised to use drills with thinned web (dubbed drill) in order to reduce friction and
reduce heat generation for large diameter holes.
10. When drilling large holes use a stepwise method: a bore of 2" for example, should
be made by drilling successively with a 1/2", 1" and then expanding the hole
further with larger diameter drills with the use of a single boring tool to dial in the final
diameter.
2. Turning Operations: And Heat Levels.
Just like mentioned from the drilling tips above, the number one challenge in turning is also maintaining proper heat levels. Turning (Lathe) require tools or inserts that have a positive geometries with ground peripheries and polished top surfaces to reduce material build up. This in turn helps improve surface finishes, we typically use PCD but a finely grained C-2 carbide is also a great option for turning operations. In roughing operation we typically (if possible) mill a slot across the diameters close to the final diameter size, this slot or slots breaks the stringing that happens in turning (breaks chips). As mentioned above if drilling in the turning operation use pecking (interrupted cut) to remove material and reduce heat.
We have gathered a list of tips or rules to follow that should help provide dimensional repeatability in your next turning operations.
1. Insert the tool width at less than the minimum diameter of the component.
2. Consider feed rates dependent on the stiffness of the stock, but typically keep chip
thickness between 0.004" - 0.010" per revolution.
3. Surface finish at the bottom of the cut is best controlled by approaching the bottom of
the cut slowly, reaching the bottom and quickly clearing the tool, use smallest width
possible to turn across.
4. Do not dwell at termination, a drag is typically experienced that alters or damages the
surface finish.
5. When turning, use single point or partial threading inserts. This results in cleaner threads
while providing ample room for chip evacuation.
6. For milling operation ( on the Lathe) use single form thread milling cutters for soft
materials and multi form for harder plastic materials.
7. Stellram grades SP4030 and SP0436 for grooving inserts are PVD coated grades with a
micro grain substrate. They are designed for machining at higher speeds and lower feeds.
These are ideal for glass or carbon filled plastics.
8. The continuous chip stream produced when turning and boring many thermoplastics can
be reduced by using compressed air powered suction systems (directly disposing the
swarf onto a container), in this way avoiding the chip wrapping around the chuck, the
tool and the work piece.
9. Machines should have a cavernous area for swarf
10. Avoid conveyor belts
11. For tubes bore one end and put a blank inside to support clamp force of jaws
12. Consider fixed pressure jaws
13. Crawford Collets are very good for plastic
14. Use tip designed for non-ferrous metals such as aluminum or brass
15. Best finish is achieved with 0.8mm radius on tool tips
16. Grind insert tips on top face to sharpen front edge
17. Use hand diamond lapper to polish grinding marks from ground tools
18. For improving tolerances, rough out large sections and leave material set for 24 hours
19. Most diameters will grow so aim for lowest dimension when setting
20. Consider doing capability studies on your machines
21. Use sliding head for small long sections
3. Threading or Tapping Operations: Hand or Machine.
All plastics are notch sensitive, what this is or means that small sharp "V" threads or features cause a material tearing problem. Use chamfers on the ends of the rod and into bores before the threading operation, this will reduce the tendency of the initial thread to tear. Coolants are often recommended when threading and tapping, remember that any tap, thread die or form tool that has tapped metal will not be sharp enough to tap plastics.
We have gathered a list of tips or rules to follow that should help reduce material tearing and dimensional repeatability in your next Threading and Tapping operations.
1. Threading is best achieved with a single point carbide insert or tool taking 4 to 5 passes
at 0.001" increments.
2. Use H-3 for smaller diameters and H-5 for larger diameters.
3. Use 0.003" to 0.005" oversized taps when threading soft plastic materials, many soft
materials expand out and close back when tapping. Always check actual cutting sizes of
the drill before tapping, most plastics close up after drilling. Thread milling on cnc
machines give better size control when the size and thread depth feature is large or
friendly enough.
4. 2 flute taps with enlarged flutes will help with chip evacuation keeping the tap clear.
5. The use of spiral taps is recommended (not straight)
6. Where possible use Rigid Tap Cycles
7. Check pilot drill sizes
8. If the tapped area must withstand heavy stresses or continued insertion and removal of
fasteners, it is best to use metal threaded inserts (steel, brass) is preferred over a tapped
plastic component. These inserts can be pressed, ultrasonically inserted, or threaded into
the plastic using self-tapping features. The structural integrity of the material ( Hard or
brittle) will determine the best insert type.
A. Most popular is self-tapping (Tappex, Spirol) be cautious though
B. If using slotted inserts, pre tap some of the thread first
C. Consider inserts with cross hole to cut
D. Avoid Heli coils in plastic
E. Some can be heat inserted but this is slower and ok for General Engineering Plastics
4. Milling and Cutting Operations: Manual and CNC.
With CNC machines climb milling is preferred or recommended over conventional milling, this is also true when machining plastics. The most difficult challenge with plastics is keeping the work piece from moving or vibrating during the operations, this results in chatter marks on the surface finishes of the components. A good way to help maintain control is to employ a vacuum system ( must have a good flat surface), double sided adhesive tape, glue or fixture clamps (these often get in the way) and a vise (be aware of stress and distortion of the work piece). We often build or machine special vise jaws, holding fixtures, board mounts, vacuum chucks and boards if the component geometry requires it. Vacuum tables are often built into CNC routers, these methods are for the manual or CNC Mill Centers used for metal work.
1. Plastics are more "elastic" so beware of part squeeze when clamped.
2. Bow more easily if clamped.
3. Less force is required to cut than metals.
4. Vacuum systems work well for Routing and light milling.
5. Double sided tape can be used for small thin parts.
6. Invest in high quality clamps for routing and milling (Lenzkes Clamping Tools).
7. Machines should have a cavernous area for swarf
8. Use mill cutters with less teeth, higher helix and good clearances
9. Avoid conveyor belts
10. For Milling machines consider vacuuming dry chips
11. Use of Vacuum plates recommended for plate parts
12. Avoid machining too much of one side of flat plates
13. Even stress out where pockets are required on one side with opposing face grooves
14. Consider using round billets in some cases to overcome small volume restrictions
We have gathered a list of tips or rules to follow that should help reduce material stress or distortion using adhesive tape and should help dimensional repeatability in your next Milling and Cutting operations.
1. Completely clean both machine surface and the plastic work piece before beginning.
2. Make sure the surface of the work piece is completely covered with one layer of tape,
avoid over lapping.
3. Place the piece of adhesive tape on the machine surface as quick as possible after
removing the protective layer, repeat this for the clean work piece as well.
4. Lightly tap the work piece down with a rubber mallet to seat securely.
5. To the remove the completed component it may be necessary to dissolve the adhesive with alcohol or solvent, if prying the part from the machine surface great care should be exercised to prevent damage, distortion, and marring or marking of the surfaces. We often use with great success plastic pry bars that are machined from softer plastics to aid in part removal.
4A. Burrs: On this note lets talk about Burrs and why to beware, a common hazard in milling is burrs. This is created when a tool reaches the end of a non supported end of the plastic work piece. To help eliminate or reduce burrs is to bring a second material to the edge of the work piece that the cutting tool can continue into, this also reduces material chipping and allow a clean cut right to the edge.
Pre-chamfering or increasing the amount of chamfering on the work piece (if possible) shifts the clean up work to the machine. To remove burrs, consider:
1. Tumbling components against each other or in media
2. Sanding
3. Polishing Wheels
4. Remove burrs by hand with specialized tools like sharp knives or rotary hook
5. Zero flute Countersink tools are recommended as they do not cut too deep or chatter
6. Hard plastics can be lightly abraded both wet and dry
7. Rotary stones can be effective on some plastics
8. Hot air good for complex General Engineering Plastics
5. Sawing Operations: Band, Circular, reciprocating and guillotine.
Sawing is typically employed in cutting raw material to near net shape for the machining application. Band saw is ideal for straight, continuous and irregular cuts. Table saw is also great for straight cuts of multiple thicknesses or thicker cross sections. Reciprocating and guillotine saws are generally suitable for cutting thermoplastics. Saw blades should be selected based on material thickness and desired surface finish. Use carbide tipped blades for the best cutting results. Here are some sawing tips:
1. Use plastic rated rip and combination blades with a 0 degree tooth rake and 3 - 10 degree
tooth set to reduce frictional heat for general sawing.
2. Hollow ground circular saw blades without set, will yield smooth cuts up to 3/4" thick.
3. Tungsten carbide blades wear well and provide optimal surface finishes, PCD blades also work very well for more abrasive plastics.
4. Set teeth (clearance between teeth side and body of cutter) far as possible to prevent material closing and trapping blade.
5. Teeth per inch (TPI) must be suited for material, soft low temp materials need a low TPI
while filled and thinner materials require a higher TPI.
Important Note: Reinforced materials like Ertalon® 66 GF30, Duratron® T4301/T4501/T5503 PAI, Ketron® HPV/GF30/CA30 PEEK, Techtron® HPV PPS, Semitron® Esd 410C and Semitron® Esd 520HR are preferably cut with a band saw with a tooth pitch of 4 to 6mm. Duratron® CU60 PBI, is preferably cut with a tooth pitch of 2 to 3mm. Do not use circular saws with these materials as edge cracks and fractures are known to acure.
Our final note here is about coolant, to maintain heat buildup temperatures, coolants are often recommended and employed during machining. Typically, it is best to avoid water-based coolants in order to achieve a premium surface finish, and petroleum-based fluids contribute to stress fractures in amorphous plastics like Altron™ PC, Sultron™ PPSU, Duratron® U1000 PEI, and Sultron™ PSU. Materials such as polyimide and Nylons can absorb up to 8% moisture resulting in extreme swelling of parts.
Note: If using coolant wash immediately in Isopropyl and pure water after machining.
For close tolerances and optimal finishes try using or employing air line air blowing with cold air guns and the use of vacuum suction to assist with chip removal, this helps to maintain a dust and odor free machining environment. We have also moved away from liquid coolants when possible to reduce the moisture absorption of most of the plastics we machine here, this dry method is not always possible but when employed it has yielded great results.
6. General Rules: Remember...
Consider rod as well as plate shapes
Machine equal to knit line
Machine pockets in intermediate steps
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
7. Annealing: Stress Relieving
Extremely close tolerance parts requiring precision flatness and non-symmetrical contour sometime require intermediate annealing between machining operations. Improved flatness can be attained by rough machining, annealing and then finishing machining with a very light cut (Kissing the Part). Balanced machining on both sides of the shape centerline can also help prevent warpage. Here are some tips for annealing:
1. When pre-machining, leave enough oversize to allow machining to final sizes after
annealing
2. Fixture parts to desired shape or flatness during the entire annealing cycle often proves
advantageous
3. Do not un-fixture until parts have completed the entire annealing cycle and are cool to the
touch
4. Make sure that temperatures are uniform and within +/- 3°C or 37°F all over the oven or
the oil bath at all times during the annealing cycle
5. Do not take short cuts
Recommended annealing for plastics:
T1: Head up time (Heat rate: 10 - 20°C/hour) or (50 - 68°F/hour)
T2: Hold time (Depends on the wall thickness: 10 minutes per mm (0.039") of part
thickness)
T3: Cool down time (Cooling rate: 5 - 10°C/hour) or (41 - 50°F/hour)
T4: Additional time required to establish normal room temperature (Depends on the wall
thickness: 3 minutes per mm (0.039") of part thickness)
Note: These are just starting points, please locate and use your materials suggested annealing guidelines. Materials and grade will vary the hold temperatures and environment used. When annealing in air, a more of less pronounced color change of the outer surface is to be expected (particularly with Nylons) the thin oxidized surface layer involved will however be removed during further machining operations of the component.
All trademarks and service marks are property of their respective manufactures. All statements, technical information, and recommendations contained herein are presented based upon tests believed to be reliable and practical field experience. The reader is cautioned, that Diversified Deigns cannot guarantee accuracy or completeness of this information. It is the customer's or user's responsibility to determine the suitability of specific products in any given application.
