Machining Cast Nylon products

Turning – Cast Nylon materials should be turned the same as free-cutting material, using high speeds of 600 to 900 ft/min 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 diameters.
In turning larger diameter pieces of Cast Nylon materials, light cuts of 1/16" to 1/8" deep and light feeds of .003" to .007" per revolution are recommended for the final pass. However, satisfactory turning results can be achieved using rough cuts up to 3/8" deep and feeds of .015" per revolution.

Sharp cutting tools with a low rake and high 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 generally adequate for turning cast nylon materials; carbide-tipped tools may be used for longer production runs if the tools are honed to a sharp edge.

Milling – Cutter speeds over 1000 feet/min with fast feed rates of 9 feet/min, and heavy cuts are commonly used for cast nylon materials. Milling 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.

For milling operations, the workpiece must be fully supported during operations on the mill. When clamping or holding is required, it is important to exercise care to prevent deformation of the workpiece.

Sawing – all Cast Nylon materials can be sawed on standard woodworking or metalworking band saws and circular saws. The blades should have widely spaced teeth to ensure adequate ship removal. 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 blade's cutting edge.

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, melting hole surface, cracking, and possible part failure.

Although properly ground, standard twist drills can be used satisfactorily, slow spiral drills with 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 lip.

A drill point angle of 90-110 ° is best for small drills, while a point angle of 118-120° is better for larger(over ½") drills. All drills should have a lip relief angle of 10 to 15 °. Standard drills previously used for metals should never be used for nylons. The use of coolants such as soluble oils or mist sprays and frequent drill pullouts (peck drilling) is 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 – ½ times the drill diameter. When drilling large or deep holes, start with a small (maximum ½" 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 hole 1" following the same procedure but using a drill speed of 400-500 RPM. Peck drill and use generous coolant for each operation.

To open the hole to the finished size, use a single-point boring tool and follow the procedure in the "turning" section.

Reaming - Whenever possible, reamers of the expansion type should be used, and reamer speeds should approximate those used for drilling (250 to 450 feet per minute). Feed rates should be between 10 and 20 mills per revolution. Since removing less than 0.0002" when reaming is difficult, leaving at least 0.005" for final reaming is best. This will provide a "bite" for the reamer and ensure accurate cutting.

Feed Rates up to 1" Dia. Drills

Feed Rates/rev	1/16" Dia.	1/4" Dia.	1/2" Dia.	1" Dia.
0.004" - 0.015"	5,000 RPM	1,700 RPM	1,000 RPM	500 RPM
0.008" – 0.016"	3,500 RPM	1,500 RPM	1,000 RPM	500 RPM
0.013"	3,000 RPM	1,000 RPM	750 RPM	400 RPM

Drill Speed/Size Chart

Drill sizes	RPM
No. 60 thru 33	5,000
No. 32 thru 17	3,000
No. 16 thru 1	2,500

Drill sizes	RPM
1/16"	5,000
1/8"	3,000
3/16"	2,500
1/4"	1,700
5/16"	1,700
3/8"	1,300
7/16"	1,000
1/2"	1,000

Drill sizes	RPM
A thru D	2,500
E thru M	1,700
N thru Z	1,300

Tapping: The tapping of cast nylon materials can be performed either by hand or by machine; however, the use of sharp taps is essential. The taps previously used on metal should never be used on nylon workpieces. In tapping, 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 of 0.010" should be suggested. Heavy cuts may be used on the initial pass, but the depth of the cut should be reduced to 0.007" on the final pass. Since nylon materials tend to memory or recovery after the die is removed, a slightly oversized die should be used for threading (see tapping section).