EUTypes of Holes in Engineering: Callout, Machining Methods & Design Tips
- Written By: Gavin Leo
- Update By: Gavin Leo
- Published:
- Updated:
Share:
Table of Content
Table of Content
A wrong hole type or an unclear callout is one of the most common reasons a machined part comes back unusable. In years of reviewing drawings at Aria, I’ve seen assemblies fail because a clearance hole was specified where a tapped hole was needed, and machinists stop production to ask what a callout actually meant.
There are 14 common types of holes in engineering: simple, through, blind, interrupted, screw clearance, tapped, threaded, counterbore, countersink, counterdrill, spotface, tapered, reamed, and overlapping holes.
This guide covers common types of engineering holes you’ll encounter in mechanical design, how to read and write their callouts, what they look like in 2D drawings and 3D views, and the machining methods and design tips that actually matter in practice.
What is a Hole in Engineering?
At its most basic, a hole is a void or opening created in a material, typically by a machining or drilling operation. But in engineering, “hole” means a lot more than that.
A hole is a designed feature with specific geometric requirements: diameter, depth, location, tolerance, and often additional characteristics like threads, countersinks, or spot faces. Each of these requirements gets communicated through a standardized callout on the engineering drawing.
Get the callout right and the machinist knows exactly what to make. Get it wrong and you’re looking at scrap, rework, or a part that doesn’t assemble.
An Overview of 14 Types of Engineering Holes
Hole type
Cross-section
Primary purpose
Simple hole
A plain cylindrical void of specified diameter. The base feature that all other hole types build on.
Through Hole
Penetrates the full material thickness. Used for fasteners, rods, fluid passages, and pin locations.
Blind Hole
Terminates at a specified depth inside the part. Used for fastener seats, pin locators, and ports that must not break through the wall.
Interrupted Hole
A drill path that crosses an internal cavity or cross-bore. Requires reduced feed rate to prevent tool deflection and breakage.
Screw Clearance Hole
Oversized to let the fastener shank pass through freely without threading. Clamping force comes from the head and nut bearing on the part faces.
Tapped Hole
Drilled then threaded with a tap so a bolt engages directly with the part material. Eliminates the need for a separate nut.
Threaded Hole
Internal thread produced by tapping, thread milling, or thread forming. Called out with thread size and tolerance class when fit is critical.
Counterbore Hole
Flat-bottomed cylindrical recess that sets a socket head cap screw flush with or below the part surface. Provides a clean face with no protruding fastener head.
Countersink Hole
Conical entry seats a flat-head screw flush with the part surface. Angle must match the fastener series: 82° for inch series, 90° for metric.
Counterdrill Hole
Stepped hole made with a larger drill to a set depth, leaving a conical shoulder from the drill point. Used for specialized fastener heads or conical-seat fluid fittings.
Spotface Hole
Minimal-depth flat recess that creates a clean bearing surface on a rough cast or inclined face. Depth is just enough to clean up the material.
Tapered Hole
Conical bore with a defined taper ratio. Self-centers and self-locks tapered shanks, pins, and pipe threads (Morse taper, NPT, BSPT).
Reamed Hole
Drill-then-ream sequence typically achieves H7 tolerance with a smoother surface finish. Required for dowel pins, bearings, and close-fit shaft locations.
Overlapping Hole
Two or more bores whose cylindrical volumes intersect. Creates complex internal geometry used in valve bodies, manifold blocks, and fluid passages.
There are two broad families of holes in mechanical engineering: Basic Hole Types (simple geometric forms) and Machined and Fastener Holes (holes designed to interface with specific hardware or require specialized machining). I’ll walk through both.
Basic Hole Types
1. Simple Hole
A simple hole is exactly what it sounds like: a cylindrical void of a specified diameter. No threading, no counterbore, no special geometry. Just a round hole with a defined size and location.
Simple holes show up everywhere, from pin locations and dowel holes to ventilation features and fluid passages. They’re the foundation everything else builds on.
The Callout Symbol of Simple Hole
A simple hole callout typically shows the diameter symbol (Ø) followed by the diameter value.
Example: In this drawing, a 20 mm diameter hole that passes through the block is called out as Ø20.00 THRU. A 16 mm diameter hole that stops 30 mm into the block is called out as Ø16.00 ↧ 30.00.
Simple Hole 2D Drawing
Simple Hole 3D Drawing
2. Through Hole
A through hole passes completely through the material from one face to the other. It’s one of the most common hole types in any mechanical assembly, used for fasteners, pins, rods, shafts, and fluid passages.
The key distinction from a simple hole description is that “through” tells the machinist (and the reader) that no depth dimension is needed because the drill exits on the far side.
The Callout Symbol Of Through Hole
Through holes have a hole callout with the diameter symbol ‘Ø’ and the words ‘THRU’.
In modern practice following ASME Y14.5-2018, if no depth is specified and the context is clear, the hole is understood to be through.
Example: Ø15.0 THRU or simply Ø15.0 with the view making it clear the hole is through.
For how through holes compare with blind holes in cost, tapping, and inspection, see blind hole vs through hole.
Through Hole 2D Drawing
Through Hole 3D Drawing
3. Blind Hole
A blind hole has a specified depth but does not break through the opposite face of the material. It terminates inside the part. Blind holes are used when you need a fastener seat, a pin location, or a fluid port without breaking through the part wall.
The Callout Symbol of Blind Hole
The callout uses the diameter symbol (Ø) and the depth symbol (↧), each followed by its value.
Example: Ø10.0 ↧ 30.0 (10 mm diameter, 30 mm deep at full diameter; the cone left by the drill point is not included in the depth)
For machining methods, tapping, and design tips, see our guide to blind holes. To compare the two most basic hole types, see blind hole vs through hole.
Blind Hole 2D Drawing
Blind Hole 3D Drawing
4. Interrupted Hole
An interrupted hole is one where the drill passes through one or more internal voids or cross-holes during machining. In other words, the hole intersects a cavity, a slot, or another hole partway through its depth.
This one’s important from a machining standpoint. When a drill bit enters an interrupted cut, it loses support on one side. The bit can deflect, wander, or in worst cases, break. It’s a situation that requires slower feeds, sharp tooling, and sometimes a pilot hole or different tool path strategy.
The Callout Symbol of Interrupted Hole
There is no dedicated ASME or ISO drawing symbol for interrupted holes. The callout follows the standard format for the hole type (through or blind), but the drawing cross-section will reveal the interrupted geometry.
Example: Ø58.5 THRU (INTERRUPTED CUT) or a general note on the drawing: CONTAINS INTERRUPTED BORE.
Interrupted Hole 2D Drawing
Interrupted Hole 3D Drawing
Machined & Fastener Holes
5. Screw Clearance Hole
A clearance hole is sized larger than the fastener shank that passes through it. The fastener doesn’t thread into this hole. Instead, it passes through freely and threads into the mating part (or a nut on the other side). The clamping force comes from the fastener head and nut bearing against the two parts.
Clearance holes come in three classes: close fit, normal fit, and loose fit. The class you choose depends on how much positional variation you can tolerate in the assembly.
Standard clearance hole sizes are listed in ISO 273 (metric) and ASME B18.2.8. Common metric sizes:
| Screw size | Close fit | Normal fit | Loose fit |
|---|---|---|---|
| M3 | 3.2 | 3.4 | 3.6 |
| M4 | 4.3 | 4.5 | 4.8 |
| M5 | 5.3 | 5.5 | 5.8 |
| M6 | 6.4 | 6.6 | 7.0 |
| M8 | 8.4 | 9.0 | 10.0 |
| M10 | 10.5 | 11.0 | 12.0 |
| M12 | 13.0 | 13.5 | 14.5 |
The Callout Symbol of Screw Clearance Hole
Clearance holes are specified by diameter, often referenced to a fastener size. For an M8 bolt:
Example: Ø9.0 THRU (M8, normal fit) or Ø8.4 THRU (M8, close fit)
Screw Clearance Hole 2D Drawing
Screw Clearance Hole 3D Drawing
6. Tapped Hole
A tapped hole is a blind or through hole that has been drilled and then threaded with a tap, a cutting tool that creates helical threads on the interior cylindrical surface. The threads allow a bolt or screw to engage directly with the part material, without a separate nut. Tapped holes are everywhere in mechanical assemblies. Any time a screw goes directly into a part (a machine housing, a bracket, a fixture plate), it’s going into a tapped hole.
Example: M20×1.5 THRU for a through tapped hole. A blind tapped hole lists both the drill depth and the thread depth, for example Ø6.8 ↧ 16 with M8×1.25-6H ↧ 12, where the 6.8 mm tap drill goes 16 mm deep and full threads reach 12 mm.
7. Threaded Hole
The terms “tapped hole” and “threaded hole” are often used interchangeably, and in many contexts they mean the same thing: a hole with internal threads. However, “threaded hole” can also refer to holes produced by thread milling (rather than tapping), or to internal threads produced by other means such as thread forming or rolling.
In precision machining applications, thread milling is often preferred over tapping for larger diameter holes, harder materials, or when thread quality and positional accuracy are critical. A thread mill produces the same thread form as a tap but removes material in a helical path rather than all at once.
When thread quality (class of fit) is critical, it’s added to the callout:
Example: M16×1.5-6H THRU (6H is a standard tolerance class for internal metric threads)
8. Counterbore Hole
A counterbore is a cylindrical enlargement at the entrance of a hole. It has a flat bottom and straight walls, and it’s sized to accept the head of a fastener (typically a socket head cap screw or a hex bolt) so that the head sits flush with or below the part surface.
The counterbore has three key dimensions: the hole diameter (for the fastener shank), the counterbore diameter (to clear the fastener head), and the counterbore depth (to sink the head to the desired level).
The Callout Symbol Of Counterbore Hole
The counterbore symbol (⌴) looks like a square-bottomed bracket, which represents the flat-bottomed recess. The callout lists the hole first, then the counterbore:
Example: Ø13.5 ↧ 30.0 ⌴ Ø23.79 ↧ 7.5
This reads as: a 13.5 mm hole, 30 mm deep, counterbored to 23.79 mm diameter and 7.5 mm deep.
Counterbore Hole 2D Drawing
Counterbore Hole 3D Drawing
9. Countersink Hole
A countersink is a conical enlargement at the entrance of a hole. Unlike a counterbore’s flat bottom, the countersink has an angled seat that matches the underside of a flat-head screw. When the screw is tightened, the conical head seats into the conical recess and the top of the screw sits flush with the part surface.
The countersink angle matters. The most common angle for standard flat-head screws is 82 degrees (inch series, ASME) or 90 degrees (metric, ISO). These are not interchangeable. Using a 90-degree countersink with an 82-degree screw leaves the head above flush. Using an 82-degree countersink with a 90-degree screw creates a line contact instead of full bearing, which can gall the part surface under load.
The Callout Symbol Of Countersink Hole
The countersink symbol (⌵) is a V shape that represents the conical seat. The callout includes the hole diameter, the countersink diameter at the surface, and the included angle:
Example: Ø9.00 ↧ 40.00 ⌵ Ø17.30 × 90°
This reads as: a 9 mm hole, 40 mm deep, countersunk to 17.30 mm diameter at the surface with a 90° included angle.
Countersink Hole 2D Drawing
Countersink Hole 3D Drawing
10. Counterdrill Hole
A counterdrill (also called a counterdrilled hole) is similar in concept to a counterbore but produced with a larger twist drill rather than a flat-bottomed boring tool. The result is a conical bottom at the stepped region rather than a flat one. It combines a short cylindrical section from the larger drill with a conical shoulder formed by the drill point, usually 118°, before the hole continues at the smaller diameter.
Counterdrill holes are used when a specific conical seat geometry is needed, often for specialized fasteners with conical heads that are different from standard flat-head screw profiles, or for fluid fittings that require a conical seat for sealing.
The Callout Symbol Of Counterdrill Hole
There is no universal standardized symbol for counterdrill holes. They are typically called out with a note specifying both diameters and the included angle:
Example: Ø20.0 THRU, Ø40.0 × 90° ↧ 20 COUNTERDRILL (a 90° included angle is specified here instead of the standard 118° drill point)
Counterdrill Hole 2D Drawing
Counterdrill Hole 3D Drawing
11. Spotface Hole
A spotface is a shallow, flat-bottomed recess machined around a hole, just deep enough to create a clean, flat bearing surface for a fastener head or washer. It’s used when the base surface of the part is rough (as-cast, as-forged, or inclined) and you need a reliable flat datum for the fastener.
The depth of a spotface is minimal, typically just enough to clean up the surface (often 0.5 to 2mm). If no depth is specified on the drawing, the machinist typically machines just enough to produce a full, clean flat. The diameter is sized to clear the fastener head or washer being used.
The Callout Symbol Of Spotface Hole
The spotface symbol is the same as counterbore (⌴) with the letters “SF” added, or it may appear as “SFACE” in a note. When no depth is specified:
Example: Ø36.0 ⌴ SF (a 36 mm diameter spotface, machined only as deep as needed to produce a clean, flat surface)
Or with a depth: Ø36.0 ⌴ SF ↧ 2.0
Spotface Hole 2D Drawing
Spotface Hole 3D Drawing
12. Tapered Hole
A tapered hole has a diameter that changes continuously along its depth, creating a conical bore. The most common applications are Morse taper holes (for tooling shanks and arbors), pipe thread connections (NPT and BSPT), and precision tapered pin holes in positioning fixtures.
Tapered holes are excellent for self-centering and self-locking applications. A tapered pin driven into a tapered hole wedges itself in place and can be removed and reinstalled repeatedly with consistent positioning. This is why tapered pins are standard practice for locating fixture components.
Taper is typically expressed as a ratio (1:20, 1:50) or as an angle per side. Morse tapers have their own standardized series with specific taper ratios.
The Callout Symbol Of Tapered Hole
Tapered holes are called out with the major diameter, minor diameter, length, and taper ratio or angle:
Example: Ø40.0 / Ø24.0 × 50.0 LONG (TAPER 8:25)
Taper ratio is the diameter difference divided by the length: (40 − 24) / 50 = 0.32, or 8:25.
13. Reamed Hole
A reamed hole is a drilled hole that has been finish-machined with a reamer to achieve a tighter diameter tolerance and better surface finish than drilling alone can provide. The reaming operation removes a very small amount of material (typically 0.1 to 0.3mm) from the drilled bore.
Reamed holes are used where close fits are required: dowel pin holes, bearing bores, shaft locations, and precision hinge pins. Standard drilled holes hold tolerances of roughly H12-H11.
Reamed holes typically achieve H7, and H6 with careful process control. This is the tolerance range used for transition and interference fits with dowel pins and shafts.
Example: Ø10 H7 THRU or Ø10 H7 ↧ 20
14. Overlapping Hole
An overlapping hole (sometimes called an intersecting hole) is created when two or more holes are positioned so that their cylindrical volumes intersect. The result is a non-cylindrical void with complex internal geometry.
Overlapping holes occur in some valve bodies, manifold blocks, and hydraulic components where fluid passages must intersect at specific angles. They also appear in some die and mold designs.
Example: Ø50.0 THRU / Ø45.0 THRU
Overlapping Hole 2D Drawing
Overlapping Hole 3D Drawing
Common Methods for Hole Machining
Every hole type I’ve described above gets made by some combination of machining operations. Here’s a practical rundown of what’s actually happening in the shop.
Drilling
Drilling is the starting point for almost every hole. A twist drill removes material by rotating and advancing axially into the workpiece. Drilling is fast and economical but produces relatively loose tolerances (IT12-IT11 typically) and a surface finish that limits its precision applications.
Reaming
Reaming follows drilling when tighter tolerances are needed. The reamer is a multi-fluted precision tool that removes a small amount of stock and leaves a very accurate, smooth bore. For dowel holes and bearing fits, reaming is standard.
Boring
Boring uses a single-point cutting tool rotated on a boring bar to enlarge and true up a drilled hole. Boring can achieve excellent roundness and straightness and is commonly used for larger diameter precision bores that exceed the practical range of reamers.
Tapping
Tapping cuts internal threads using a tap: a hardened, fluted cutting tool with the thread form ground into it. Tapping can be done by hand or by CNC with a synchronized spindle. Thread forming (cold forming rather than cutting) is an alternative that produces stronger threads in softer materials by displacing rather than removing material.
Thread milling
Thread milling uses a rotating thread mill tool to generate the thread form in a helical path. It’s slower than tapping but more flexible: one tool can cut multiple thread sizes, and it can be used in materials that are difficult or impossible to tap conventionally.
Counterboring
Counterboring uses a flat-bottomed end mill or a dedicated counterbore tool. The through hole is drilled first, and then the counterbore tool pilots in the existing hole to produce the larger stepped recess.
Countersinking
Countersinking uses a countersink cutter (a conical cutter with the appropriate included angle) to create the angled entry. The through hole is drilled first, then the countersink is run in to the required diameter at the surface.
Design Tips for Engineering Holes
After years of designing parts and watching them come back from the shop, I’ve collected a few rules I stick to.
Size your holes to standard tooling
Drill bits come in standard sizes. If you design a 7.3mm hole when a 7.5mm hole would also work, you’ve just created a special tooling requirement. Use standard drill series sizes wherever the function allows it.
Think about depth-to-diameter ratio on blind holes
Drilling a hole much deeper than 3-5 times the diameter without peck drilling cycles is asking for chip packing and drill breakage. For very deep holes (greater than 10x diameter), you’re into gun drilling territory, and that changes your manufacturing approach completely.
Never design to minimum wall
I’ve seen drawings that calculate the absolute minimum wall between two holes and then call it out exactly. Leave margin. A 0.5mm minimum wall on paper becomes a scrapped part when drilling tolerances stack up.
For tapped holes, specify both thread depth and drill depth
The drill depth needs to be deeper than the thread depth to allow tap runout. As a rule of thumb, make the drill depth 3 to 5 thread pitches deeper than the full thread depth. Spiral flute taps with a short chamfer need less extra depth, while plug taps and spiral point taps need more.
Consider access for tooling
A tapped hole in a pocket with 8mm clearance around it looks fine in CAD. In the shop, the tap holder needs to fit in that pocket too. Build enough clearance for the tooling that will make the feature.
Conclusion
Hole callouts are where many drawing errors start. Aria’s engineering team reviews hole types, depths, thread callouts, and tool access as part of every CNC machining quote, so problems are caught before production starts.
Custom Quality Parts By Aria
Send your specs. We’ll get back with a quote in 12 hours.
