< Back to Articles

Machining Cast Nylon products

Machining Cast Nylon
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. Satisfactory turning results can be achieved, however, using rough cuts up to 3/8” deep and feeds of .015” per revolution.

Sharp, honed tools with 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 very sharp edge.


Milling – Cutter speeds in excess of 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 assure adequate ship 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 blade.


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 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 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. Use of coolants such as soluble oils or mist sprays, together with frequent drill pullout (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 – 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 the hole 1” following the same procedure but 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 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 it is difficult to remove less than 0002” 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 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          1,700RPM          1,000 RPM       500 RPM

                                      1,500 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

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                  

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” is 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 have a tendency toward memory or recovery after the die is removed, a slightly oversized die should be used for threading (see tapping section).

Title: Machining Cast Nylon products
Description: Infortmation on how to turn, mill, drill, ream, tap, and tread Cast Nylon.
Published: 5/28/2008
Last Edited: 9/18/2013
42 users found this article useful. Was this article useful to you?

Information disclaimer:

The information contained in this article is for general information purposes only. The information is provided by United States Plastic Corp. and while we endeavor to keep the information up to date and correct, we make no representations or warranties of any kind, express or implied, about the completeness, accuracy, reliability, suitability or availability with respect to the website or the information, products, services, or related graphics contained on the website for any purpose. Any reliance you place on such information is therefore strictly at your own risk.

In no event will we be liable for any loss or damage including without limitation, indirect or consequential loss or damage, or any loss or damage whatsoever arising from loss of materials, time or profits arising out of, or in connection with, the use of this information.