Machining thermoplastics

Think & Tinker, Ltd.
P.O. Box 1606, Palmer Lake, CO 80133
Tel: (719) 488-9640, Fax: (866) 453-8473
Sales: Sales@ThinkTink.com, Support: Support@ThinkTink.com

Think
&
Tinker
Ltd.

SkypeMe at
"thinkntink"

Machining thermoplastics

Cutting thermoplastics often requires a tighter optimization of feeds and speeds than encountered in most other machining operations. Problems encountered include poor swarf (cutting debris) extraction, reattachment of cut material, melting, and part distortion. In addition, the direction of cut (conventional or climb milling) can have a profound effect on the final edge quality and dimensional fidelity. The effects of these parameters can be somewhat mitigated by matching the flute geometry to the shear requirements of the material being cut. Nonetheless, accurate, reliable results can only be achieved by considering the effect of every machining parameter and tuning each one with respect to the other. If a high level of precision is required, the same techniques used in zero-glue-line inlay should be adopted.

The photomicrographs on the left dramatically demonstrate the importance of optimizing spindle RPM (speed) , feed rate and cutter geometry to the material being cut. The material in question is a vacuum formable thermoplastic used in the manufacture of medical appliances. Although cut with a sharp new tool (as shown by the clean, square edge profiles), there was enough mismatch between the material properties, feed, speed and/or cutter geometry that significant amounts of the material being cut melted and flowed into the filigree ribbons shown growing from the external edges of the part. Burrs of this type are usually the result of the generation of excessive heat combined with poor swarf extraction during a machining operation.

Machining parameters:

Feed - 36 in./min. (914 mm/min.)
Speed - 27,000 RPM
Cut direction - conventional
Cutter - 1.5 mm dia. 2 flute, up-cut
Depth of cut - 0.8 mm

A spindle speed of 27KRPM, with a feed rate of 36 in./min. (although a bit low) should have produced a smooth, clean, burr-free cut in this type of material. The formation of the melted burrs is a pretty good indicator that either the bit was very dull or the flute geometry was tuned for a much harder material (e.g. brass or silver).

A reasonable facsimile to the edge quality and burr formation was achieved with a 1/16 in. (1.59 mm) 2 flute soft media cutter (MM208-0625-031F).

Machining parameters:

Feed - 5 in./min. (127 mm/min.)
Speed - 27,500 RPM
Cut direction - conventional
Cutter - 1.59 mm dia. 2 flute, up-cut
Depth of cut - 0.8 mm

As can be see in the photomicrographs to the right, significant burr formation has occurred as a result of melting and reattachment of cutting debris.

This test cut was made using a high-shear bit optimized for cutting plastics. The flute geometry matches the material shear requirements so well that it was necessary to slow the feed down to a crawl to inhibit swarf extraction and initiate melting and reattachment of the cut material.

This is a good place to point out that, more often than not, a high feed rate is better than a low one when cutting materials that melt. You can think of the flutes of a rotary cutter as constituting a spiral screw pump (Archimedes screw). As the bit rotates and moves forward, new material is cut, forcing previously cut debris up the flutes and out of the kerf (slot). If the feed rate is too low, the debris stays in the flutes too long, gets hot, melts, and re-adheres to the parent stock.

The two sets of photos below, when contrasted with the samples above, clearly demonstrate that increasing the feed rate can virtually eliminate burr formation. With the reduction of heat, the edge quality significantly improves as does the accuracy of the cut. Although the final test was run at 30 in./min., an evaluation of the stress on the cutter indicates that feed rates in excess of 100 in./min. could be used on this material with no impact on edge quality or cutter life (assuming that the CNC system is rigid enough to sustain such feed rates).

mouse over
for larger image

Machining parameters:

Feed - 10 in./min. (254 mm/min.)
Speed - 27,500 RPM
Cut direction - conventional
Cutter - 1.59 mm dia. 2 flute, up-cut
Depth of cut - 0.8 mm

Machining parameters:

Feed - 30 in./min. (762 mm/min.)
Speed - 27,500 RPM
Cut direction - conventional
Cutter - 1.59 mm dia. 2 flute, up-cut
Depth of cut - 0.8 mm

mouse over
for larger image

As shown above, for a given spindle RPM (speed) and cutter geometry, the edge quality achieved when machining thermoplastics depends heavily on feed rate. Generally speaking, the faster you go (higher feed rate) the better. Extensive testing has shown that the best feed rate , in terms of edge quality and cutter life, for most of these materials is only 25% lower than the feed rate at which the tool breaks.

Machining parameters - How you cut and shape thermoplastics depends a great deal on what kind of material you are dealing with. Determining a comprehensive cutting strategy is virtually impossible because the properties that most affect machinability (e.g. melting point, hardness and abrasiveness) can vary all over the map. Generally speaking you will need to use a cutting tool with a high-shear flute geometry, lots of flute volume (1 or 2 flute tools work best), and a high enough helix angle to insure fast, efficient chip removal. Recommended total chip loads (TCL) for selected materials are listed below. The table assumes that you are plunging the bit to it's full cutting depth (DOC). (NR = Not Recommended)

Total Chip Loads (in./rev)	Cutter Diameter
Material	0.0156	0.0200	0.0313	0.0469	0.0625	0.0938	0.1250
Teflon© (1 flute)
ABS (2 flute)
polyethylene (LDPE, 2 flute)
polyethylene (HDPE, 2 flute)
polypropylene
PVC (2 flute)
Plexiglas© (2 flute)
Lexan© (2 flute)
polycarbonate (2 flute)

Established 1990

On the web 1994

Payment Processing