What Is Drilling?

For drilling operations on acrylic sheets, any commercially available power-driven equipment is suitable. This includes, but is not limited to, portable hand drills, bench drill presses, lathes, automated multi-spindle drilling units, CNC routers, and machining centers.

The market offers various drill bits specifically designed for plastic materials. These bits are typically made from high-speed steel (HSS), cobalt alloys, carbide-tipped HSS, or solid carbide. Additionally, standard metal-working HSS twist drills can be used for acrylic materials with appropriate modifications.

Standard metal-working drill bits are designed to actively cut into metal with aggressive feeding. If used on acrylic materials without any modifications, these bits will cause chipping, notching, and other damage to the sheet. Therefore, these bits must be reground to process plastic in a "scraping" rather than "sharp cutting" manner, thereby preventing the material from being punched through.

When adapting standard metal twist drills for plastic processing, three main aspects must be considered:

Point Angle

The point angle of standard drill bits typically ranges from 118° to 130°. This tip angle must be ground to 60° to 90°. This helps the drill bit enter and exit the acrylic sheet smoothly, thus preventing edge chipping. Larger point angles (e.g., exceeding 90°) typically cause cracking and blow-out when the drill bit exits the sheet.

For most acrylic sheet drilling operations, a 90° point angle drill bit is recommended. A 90° point angle produces smaller chips that are easier to evacuate, helping to reduce material melting and improve hole quality. Special attention is required during entry and exit. Drill bits with a 60° point angle are also commonly used, particularly for holes with diameters of 1/2 inch and above.

The cutting edge must be ground flat to maintain a rake angle between 0° and 4°. The cutting edge modified in this way will "scrape" the acrylic rather than "chisel" it.

Rake Angle

The surface behind the cutting edge must be ground to provide a clearance angle of 12° to 15°. This back clearance reduces the contact area between metal and plastic, thereby reducing heat buildup. This modification is typically standard on high-quality twist drills.

Clearance Angle / Back Relief

The helix angle of a drill bit is the angle between the cutting edge and a vertical line along the drill bit's centerline. Drill bits with moderate helix angles facilitate chip evacuation and are therefore recommended for plastic drilling. A helix angle that is too small will impede chip evacuation and increase melting risk. A helix angle that is too large may cause cracking at the hole edges. The typically recommended helix angle is 15° to 30°.

Helix Angle

Drill bit geometry is critical to hole quality because it directly affects chip size and chip evacuation efficiency. Larger diameter drill bits and drill bits with smaller point angles produce larger chips. If the hole depth (H) is less than the drill bit diameter (D), large chips can be evacuated easily. As hole depth increases (i.e., H > D), evacuation of large chips becomes difficult due to the very small clearance between the drill bit and hole wall. Increasing the drill bit point angle can reduce chip size, thus facilitating chip evacuation. However, as previously mentioned, if the point angle is too large (greater than 90°), the drill bit may cause blow-out and chipping when exiting the acrylic.

When performing drilling operations, be sure to follow the safety recommendations of equipment and material manufacturers.

When drilling acrylic sheets, a large amount of heat is generated due to the extremely small clearance between the drill bit and hole wall, combined with difficult chip evacuation. Additionally, acrylic's relatively low thermal conductivity and high thermal expansion coefficient cause the material to expand, further exacerbating friction. If left uncontrolled, these factors can lead to material melting and adhesion, affecting hole quality. Therefore, minimizing generated heat and quickly removing chips is crucial.

The workpiece should be firmly clamped to the worktable. Best practice is to use another piece of acrylic, other thermoplastic sheet, or medium-density fiberboard (MDF) as a backing plate support, allowing the drill bit to continue drilling into solid material as it penetrates the bottom surface. This effectively prevents bottom surface chipping.

When beginning the drilling motion, a slower feed rate should be used to allow the drill bit to enter the material smoothly; when the drill bit is about to exit the bottom surface, the feed rate should also be reduced to prevent edge chipping.

Proper drilling conditions are a combination of spindle speed (RPM) and feed rate (IPM). The following two parameters are typically used to determine these conditions:

SFM (Surface Feet per Minute): The speed at which the drill bit's cutting edge strikes the material.

IPR (Inches Per Revolution): The amount of material removed per revolution of the drill bit, also known as chip load.

Although SFM and IPR cannot be directly set on manual drilling equipment, they can be used to determine spindle speed (RPM, revolutions per minute) and feed rate (IPM, inches per minute). If optimal SFM and IPR values have been determined, the following formulas can be used to determine equipment settings:

Recommended Drilling Conditions

For acrylic drilling, the recommended SFM and IPR values are shown in the following table:

Drill Diameter (inches)	SFM (Surface Feet/Minute)	IPR (Inches/Revolution)
1/16	20 - 160	0.001
1/8	20 - 160	0.002
1/4	20 - 160	0.004
3/8	20 - 160	0.006
1/2	30 - 90	0.008
3/4	30 - 90	0.010
≥ 1	30 - 90	0.012 - 0.015

Charts showing larger diameter drill bits require lower SFM

As shown in the table above, larger diameter drill bits require lower SFM. This is to ensure smooth, vibration-free drilling operations, as large drill bits more easily grab the material. Therefore, the feed rate typically must be reduced to prevent edge chipping, while spindle speed must be reduced to prevent material melting.

For cases where H > D, "peck drilling" should be employed-that is, drilling in segments and periodically withdrawing the drill bit from the material to clear chips.

Manual drilling operations should employ lower speeds and feed rates than automated or CNC drilling. While considering drill bit diameter, material thickness, and cooling capacity, deep hole drilling should employ peck drilling to reduce melting. Since manual drilling makes precise feed rate control difficult, after determining the correct RPM, the hole's surface finish can be used as a guide for feed rate. If the material chips, the feed rate is too fast and must be reduced. If the material melts, the feed rate is too slow (causing frictional heat) or RPM is too high, and adjustments must be made.

The shape of chips produced during drilling can serve as a reference for judging drilling conditions:

Optimal Conditions: Hole surface is smooth, chips appear as smooth, continuous ribbons.

Feed Rate Too High or RPM Too Low: Chips are powdery and discontinuous, cutting is uneven.

Feed Rate Too Low or RPM Too High: Chips are melted and clumped, hole walls show melting marks.

When conditions permit, air or liquid coolant should be used whenever possible. Coolant can effectively reduce generated heat, thereby improving hole quality. At specific hole depths and sizes, coolant is a necessary means of preventing melting.

General Rule: When hole depth (H) exceeds drill bit diameter (D) (e.g., when D=0.250", coolant should be used if H>0.250"), or when hole diameter is greater than or equal to 1/2 inch (D ≥ 1/2"), coolant should be used.

Choice: Cold air guns provide good cooling effect and are cleaner to use. However, liquid coolants provide stronger cooling because the liquid can flow along the drill bit to the hole depth, resulting in better hole finish. Water, kerosene, mineral oil, or other compatible solvents can all be used.

For holes that may bear the forces of screws or bolts, a countersink tool should be used for deburring. Zero-flute countersinks are very suitable for countersinking and deburring operations on acrylic sheets. If a countersink tool is unavailable, a drill bit larger than the hole diameter can be used to deburr the rough edges on the exit side of the hole (the side where the drill bit exits the sheet).

Circuit board drilling is a special case, using automated machines to drill thousands of tiny holes at extremely high speeds. This requires specially designed drill bits. Recommended feed rates and RPM can be referenced from relevant charts.

Circuit board drilling feed rate and RPM recommendation charts

To drill holes with diameters larger than 1 inch (25.4 mm) in acrylic sheets, a circle cutter can be used. The tool must also be modified to suit acrylic's material characteristics: the cutting tip must process acrylic in a scraping manner rather than chiseling.

For optimal cutting results, follow these recommendations:

The circle cutter and cutting tool itself must be securely fixed.

The cutting tool's extension length need only reach the required cutting depth.

The acrylic sheet must be adequately supported and clamped to prevent bending or vibration during cutting.

The material should be placed as close to the tool as possible to reduce the tool's travel distance.

Recommended spindle speed is between 400-600 rpm.

A slow, steady feed rate is crucial for obtaining clean, smooth holes.

When the hole is complete and the "center plug" drops out, it's best to turn off the drill press without removing the tool to prevent the tool from causing hole chipping during withdrawal.

A small amount of water mist is recommended for cooling to keep the tool and plastic at low temperature, and also serve as a cutting lubricant.

Note: Circle cutters should only be used on bench drill presses, and the acrylic sheet must be firmly clamped to the machine's worktable. The drill press provides uniform pressure and constant positioning, which are critical for safely drilling high-quality holes. Never attempt to use a circle cutter with a handheld drill.

The preceding sections primarily concerned controlled production and workshop applications. However, sometimes drilling must be performed in the field (e.g., at a construction site), where precise speed and feed control is limited. In such cases, the following drill bit recommendations may be helpful.

Several drill bit geometries that can be successfully used are described below, although most of these cannot produce a smooth surface finish on the hole's inner diameter. These drill bits must also follow the previously mentioned backing plate support and cooling requirements.

Spade Bit (1-1/2" to 2"): Use advanced designs, such as types with outer rim pivot points, which help with alignment and provide smooth breakout when the drill bit exits the material.

Brad Point Bit (1/8" to 1"): This design is similar to a twist drill but with an improved tip and pivot point similar to a spade bit. It has a helical flute design that helps pull out chips, superior to general spade bits.

Step Drill (1/8" to 1/2"): Can be used for sheets up to 0.118" (3 mm) thick to achieve multiple hole diameters with a single drill bit. Use requires maximum support behind the sheet to prevent cracking.

Hole Saws with Center Pilot Drill (3/4" to 6"): Cooling is required during cutting to prevent stress buildup within the sheet. They produce poor hole inner surface finish. Suitable for rough passage holes for HVAC, plumbing, or wiring installation.

Hole center distance from edge and hole diameter to bolt diameter relationship diagram

When drilling holes for point fastener support of sheets, two rules must be followed:

Hole Diameter Size: The bolt hole diameter should be at least 2 times the bolt diameter. This provides sufficient clearance for thermal expansion and moisture expansion/contraction.

Edge Distance: The distance from the hole center to the sheet edge should be at least 1.5 times the hole diameter.