Machining Guidelines - Drilling

Drilling plastic materials requires precise techniques and proper tooling to avoid common issues like melting, chipping, and crazing. Unlike metals, plastics have low thermal conductivity and tend to retain heat generated during drilling, making proper speeds and feeds critical for successful results.

Key Considerations for Drilling Plastics:

• Point Geometry: Use specialized point angles (90-118°) depending on the plastic type. Standard 118° points may cause grabbing in some materials.
• Clearance Angle: A 12-15° clearance angle reduces friction and heat buildup during drilling.
• Cooling: Use compressed air cooling for most applications. For deeper holes or heat-sensitive materials, water-soluble coolants may be necessary.
• Peck Drilling: Recommended for deeper holes to allow chip evacuation and prevent heat buildup.
• Feed Rate: Maintain consistent, moderate feed pressure to prevent melting or material piling at the hole entry/exit.

The table below provides specific drilling parameters for different plastic materials based on their machinability ratings and physical properties.

Threading should be done by single point using a carbide insert and taking four to five 0.001" passes at the end. For tapping, use the specified drill with a two-flute coated tap. Remember to keep the tap clean of chip build-up. Use of a coolant during tapping is also suggested.

Use of a coated tap will create radii at the root of the threads resulting in a stronger and tougher thread which is less prone to cracking from over-torqueing.

Use of thread cutting and thread forming screws is not recommended as tremendous stresses around the hole may likely cause cracking.

Drilling Guidelines by Hole Size:

Small diameter holes (1/32" to 1" or 1mm to 25mm) - High speed steel twist drills are generally sufficient for small holes. To improve swarf removal, frequent pull-out (peck drilling) is suggested. A slow spiral (low helix drill will allow for better swarf removal.

Large diameter holes (1.0" or 25mm and larger) - A slow spiral (low helix) drill or general purpose drill bit ground to a 118° point angle with 9° to 15° lip clearance is recommended. The lip rake should be ground (dubbed off) and the web thinned.

Special Considerations for Notch Sensitive Materials:

A two-step process using both drilling and boring can be used on notch sensitive materials such as Ertalyte^® PET-P, Torlon^® PAI, Vespel^® PI, Celazole^® PBI and glass or carbon reinforced products. This minimizes heat build-up and reduces the risk of cracking.

1. Drill a 1" diameter hole using an insert drill at 500 to 800 rpm with a feed rate of 0.005" to 0.015" per revolution.
2. Bore the hole to final dimensions using a boring bar with carbide insert with 0.015" to 0.030" radii at 500 to 1,000 rpm and a feed rate of 0.005" to 0.010" per revolution.