MACHINING OF CAST NYLONS
The following are recommended machining
instructions for cast nylon materials:
Turning: Materials should be turned the
same as a free-cutting material, using high speeds of 600 to 900 surface speed,
with heavy roughing cuts at feed rates per revolution of 0.004" to
0.010" for smaller diameters, and 0.003" to 0.007" for larger
In turning large diameter pieces of
material, light cuts of 1/16" to 1/8" deep and light feeds of
.003" to .007" per revolution are recommended for the final pass.
Satisfactory turning results can be achieved using roughing cuts up to 3/8"
deep and feeds of .015" per revolution.
Sharp, honed tools with high rake and
clearance angles are suggested to minimize cutting forces, reduce heat build-up,
and obtain the best results when turning, boring, facing, or milling. Tools made
of high speed tool steel are adequate for turning, but carbide-tipped tools may
be used for longer production runs if they are honed to a very sharp
Milling: Cutter speeds in excess of 1000
ft/min with fast feed rates of nine ft/min and heavy cuts are commonly used.
Cutters designed for light metals can be used, but fly cutters generally perform
better because of swarf removal. Milling cutters must be sharp and have high
positive cutting angles. The workpiece must be fully supported during all
operations on the mill. When clamping or holding is required, it is important to
exercise care to prevent deformation of the workpiece.
Sawing: Materials can be sawed on standard
woodworking or metalworking band saws, and circular sawsThe blades should have
widely spaced teeth to assure adequate chip removal. In order to avoid excessive
heat build-up and possible binding of the saw, blades should have enough set to
accommodate the tendency of nylons to close-in behind the cutting edge of the
Drilling: Drilling is the most difficult of
all nylon machining operations due to the confined space in which drills operate
and the poor heat conduction of nylons. Proper tooling and procedures, however,
will eliminate problems such as gumming, melted hole surface, cracking, and
possible part failure.
Although properly ground, standard twist
drills can be used, slow spiral drills with their larger flute areas provide a
clearer path for chip flow. For best results, use a new drill and grind the tip
to thin the web area and provide a 0-5 degree positive rake angle at the cutting
A drill point angle of 90° to 110°
is best for small (under 1/2") drills, while a point angle of 118° to
120° is better for larger (over 1/2" drills). All drills should have a
lip relief angle of 10° to 15°. Drills previously used for metals should
never be used for nylons. Coolants, such as soluble-oils or mist sprays,
together with frequent drill pull-out (peck drilling) are essential to
successful drilling operations. A good guide for peck drilling is to pull the
drill out of the hole after drilling to a depth not more than 1-1/2 times the
drill diameter. When drilling large or deep holes, start with a small (maximum
1/2" diameter) hole drilled at a speed of 800 to 900 rpm and a feed rate of
.005" per rev. The web area and cutting lip must be ground to prevent
"grabbing" and stress cracking. Open the hole to 1" following the
same procedures using a drill speed of 400-500 rpm. Peck drill and use generous
amounts of coolant for each operation. To open the hole to finished size, use a
single point boring tool and follow the procedures in the "turning"
Reaming: Whenever possible, reamers of the
expansion type should be used, and speeds should approximate those used for
drilling (250 to 450 ft per min). Feed rates should be between 10 and 20 mils
per revolution. Since it is difficult to remove less than .002" when
reaming, it is best to leave at least .005" for final reaming. This will
provide a "bite" for the reamer and will assure accurate
Tapping: Can be performed either by hand or
by machine, however, the use of sharp taps is essential. Taps previously used on
metal should never be used. High speed oversize taps, such as H-3 oversize, can
be used for smaller diameters, and H-5 oversize for larger diameters. Any high
speed tap used should be oversized by 0.002" to 0.005".
Threading: As in tapping, dies must be
sharp and should never have been used on metal. Threads can be cut with any
conventional method, but dies must be well backed-off to avoid non-cutting
surface contact with the workpiece.
Threads may be cut with a single point
tool. Light cuts of less than 0.005" should be avoided, and a maximum cut
of 0.010" is suggested. Heavy cuts may be used on the initial pass, but the
depth of the cut should be reduced to 0.007 inches on the final pass. Since
nylon materials have a tendency toward memory or recovery after the die is
removed, a slightly oversize die should be used for threading.
For more information, contact, Cast
Nylons Ltd., 4300 Hamann Pkwy., Willoughby, OH 44094, 800-543-3619, FAX
440-269-2323, www.castnylon. com.