Blind holes are one of the most commonly misspecified features in CNC machined parts. When you submit an RFQ without a depth callout, a bottom geometry type, or a thread depth separate from drill depth, the factory guesses - and the wrong part only surfaces at assembly.
A blind hole is a machined hole that stops at a specified depth inside a part instead of passing through to the opposite face. On a CNC drawing, a blind hole should define the hole diameter, controlled depth, bottom geometry, thread length if tapped, and any tolerance or surface requirement.
Blind holes matter because small drawing gaps can lead to wrong tooling, incorrect thread engagement, assembly failure, or rejected parts. The most common issues are missing depth callouts, unspecified drill-point or flat-bottom geometry, and unclear thread details on tapped blind holes.
This guide explains what blind holes are, how they differ from through holes, how CNC shops machine and inspect them, and what procurement teams should specify before sending an RFQ to a CNC machining factory in China.
A blind hole is defined as a drilled or machined cavity that enters a workpiece from one face and stops at a specified depth, leaving the opposite face intact. Unlike a through hole, it has only one opening. The closed end (sometimes called the blind bore bottom) varies in shape depending on the cutting tool: a standard twist drill leaves a conical point at approximately 118 degrees, while a flat-bottom drill or end mill produces a planar surface.
The engineering purpose extends well beyond simply not penetrating the part. Blind holes preserve structural mass, seal internal fluid channels, allow hidden fastening, and keep exterior surfaces clean. You'll find them in pump housings, battery enclosures, precision machine frames, automotive engine blocks, and consumer electronics - anywhere internal attachment or sealing is required without visible hardware on the outside.
These two hole types affect tooling selection, programming, cost, and inspection difficulty. The table below covers the critical parameters:
|
Parameter |
Blind Hole |
Through Hole |
|
Depth |
Terminates within the material |
Passes completely through |
|
Bottom geometry |
Conical (118 degrees) or flat |
Open exit face |
|
Chip evacuation |
Constrained - requires peck drilling or coolant |
Unrestricted |
|
Thread engagement |
Limited by blind depth |
Full material thickness |
|
Structural integrity |
Higher - preserves material mass |
Lower - removes more material |
|
Inspection |
Requires bore gauge or CMM |
Direct measurement |
|
Coolant delivery |
Pressure-fed recommended |
Standard flood acceptable |
|
Relative machining cost |
Higher |
Lower |
Blind holes take longer to program, require more controlled cutting strategies, and are harder to inspect than equivalent through holes. The CNC machining cost impact per feature depends on material, depth, and complexity. But the cycle time and inspection overhead are real factors in any RFQ, particularly at higher volumes.
Not all blind holes are the same feature. The type you specify determines which tooling the factory uses, how they program the tool path, and what the bottom geometry looks like. Getting the type wrong on a drawing is a common source of parts that fail assembly.
|
Type |
Bottom Geometry |
Primary Use Case |
Tooling |
|
Standard drilled |
Conical, 118-degree point |
General fastener retention, clearance holes |
Twist drill |
|
Flat-bottom |
Planar |
O-ring sealing, precision counterboring, hydraulic ports |
Flat-bottom drill or end mill |
|
Threaded (blind tapped hole) |
Conical + partial thread runout |
Internal thread for fasteners or inserts |
Twist drill + tap |
|
Reamed |
Conical or flat, tight tolerance |
Precision dowel pin location, bearing bores |
Drill + reamer |
|
Counterbored |
Two-diameter stepped flat bottom |
Socket head cap screws flush with surface |
Drill + counterbore cutter |
|
Undercut |
Internal groove below entry diameter |
Snap-fit joints, retaining rings |
T-slot or undercutting end mill |
Worth noting: the flat-bottom type is often overlooked on drawings. If your design requires full thread engagement from the very bottom of the hole - for example, a hydraulic port plug that must seat against a flat face - you need to call out flat-bottom geometry explicitly. A standard drilled hole won't achieve that; the conical tip eats into your usable thread depth.
A blind hole is called out on a technical drawing using two symbols placed in sequence after the feature's diameter. The diameter symbol (ø) states the hole size, and the depth symbol (↧) states how deep the hole should go.
Example callout: ø6.0 ↧18.0 means a blind hole 6 millimetres in diameter and 18 millimetres deep.
For a threaded blind hole, the callout extends further. A typical metric example: ø5.0 ↧20.0, M6x1.0 ↧15.0. This tells the factory to drill a 5.0mm pilot hole to a depth of 20mm, then tap an M6x1.0 thread to a depth of 15mm - leaving 5mm of unthreaded drill depth below the thread for chip clearance.
The distinction between drill depth and thread depth is one of the most frequently missed details on procurement drawings. If you only call out the thread depth and omit the drill depth, the factory has to assume - and their assumption may not match your assembly requirements.
Sidenote. In Geometric Dimensioning and Tolerancing (GD&T), a positional tolerance callout for a blind hole applies to the axis of the hole, not the bottom surface. If you need the bottom surface to be flat and within tolerance, add a flatness callout separately.
The depth-to-diameter ratio (D:d) is the single most important design constraint for blind holes. It directly affects tool deflection, chip packing, heat buildup, and whether the part is machinable without specialty tooling.
|
D:d Ratio |
Machining Category |
Tooling Type |
Practical Notes |
|
Up to 3:1 |
Standard |
Standard twist drill or end mill |
Routine; any CNC machine shop handles this |
|
3:1 to 5:1 |
Intermediate |
Extended-reach drill, peck drilling required |
Slower cycle time, needs pressure coolant |
|
5:1 to 10:1 |
Deep hole |
Gun drill or BTA drill |
Specialty process; increases cost and lead time significantly |
|
Above 10:1 |
Not recommended |
No standard tooling |
Redesign required in most cases |
The 3:1 rule is the number to remember for standard CNC machining. If your blind hole is 8mm in diameter, keep the depth at or below 24mm. Push past 3:1 without specifying the right tooling and you're asking the factory to make a judgment call - which increases the risk of tool breakage, diameter drift, and poor surface finish at the bottom of the hole.
If your design genuinely requires a deeper hole, flag it explicitly in your drawing notes and discuss it with your supplier before production starts.
Blind holes are machined using drilling, end milling, or boring operations, depending on the required diameter, bottom geometry, and surface finish. The drilling process for a standard blind hole follows a specific sequence: a spotting drill or center drill establishes the entry point precisely, then a twist drill cuts to the required depth.
The challenge that separates blind hole drilling from through hole drilling is chip evacuation. In a through hole, chips fall out freely.
In a blind hole, they accumulate at the bottom. As the hole fills with chips, friction increases, tool temperature rises, and the drill can deflect from its intended path.
Peck drilling is the standard response. The drill advances to a programmed depth, retracts fully to clear chips and allow coolant in, then advances again.
For deep holes - particularly above a 3:1 D:d ratio - peck drilling isn't optional. Skipping it to save cycle time is a reliable way to break tools and scrap parts.
Pressure-fed coolant through the tool spindle is the preferred method for controlling heat in blind holes, especially in stainless steel 304, titanium Ti-6Al-4V, and other materials that work-harden under heat. Conventional flood coolant doesn't reach the bottom of deep blind holes effectively.
Tapping a blind hole - creating internal threads inside a cavity that doesn't go through - requires more precision than tapping a through hole, for one simple reason: the tap has nowhere to go once it hits bottom.
The minimum drill depth for a tapped blind hole is typically calculated as: Drill depth = Thread depth + (1.5 x thread diameter) + tap lead.
The 1.5x diameter buffer provides chip clearance at the bottom of the hole. Without it, chips pack under the tap, increase torque, and break the tool. Tap breakage in a blind hole is one of the more time-consuming problems in machining - extracting a broken tap often costs more than the original part.
Three tap types apply to blind holes:
Sidenote. As a practical rule, keep thread depth at or below 2x the thread diameter in blind holes. Beyond 2x, the additional thread engagement adds very little to the joint's strength and significantly increases the risk of tap breakage.
Blind holes retain fluid - and that retained fluid can destroy a housing during assembly. It's a failure mode that doesn't appear in most machining guides, and it should.
Coolant, cutting oil, and hydraulic fluid all collect at the bottom during machining and part washing. When you insert a fastener into a fluid-filled blind hole, the fastener acts as a piston.
The trapped fluid has nowhere to go. If the hole walls are rigid - as in an aluminium engine block, a cast pump housing, or a hydraulic manifold - the hydraulic pressure generated by tightening the fastener can crack the surrounding material.
This isn't a theoretical problem. For example, EngineLabs documents exactly this failure in performance engine building: “When a stud or bolt is threaded in place, this can cause a hydraulic situation that will also instantly crack the block.” The same physics apply to any rigid housing with blind threaded holes.
The fix is simple: blow out every blind hole with compressed air before assembly. If the part has been through a coolant bath or washing station, treat every blind hole as potentially fluid-filled. One extra second of air before threading a fastener saves a scrapped housing.
When ordering CNC parts with blind holes, specify the hole diameter, depth, thread details, bottom geometry, surface finish, and position tolerance on the drawing. These details help the supplier choose the right tooling, machining strategy, and inspection method before quoting or producing the part.
Include the following in your RFQ drawing:
The most common blind hole drawing issues are missing drill depth on tapped holes and unclear bottom geometry on sealing features. Both can lead to incorrect tooling choices, poor thread engagement, leakage, assembly failure, or rejected parts.
If you are sourcing CNC machined parts with tight blind hole requirements, Haizol can route your RFQ to verified factories matched to your process needs across CNC machining services, including milling, turning, and precision drilling.
A through hole passes completely through the workpiece from one face to the other. A blind hole terminates at a controlled depth inside the material. Through holes are easier to drill and tap because chips fall freely; blind holes require peck drilling and careful chip management because the bottom is enclosed.
A blind hole is called out using the diameter symbol (ø) followed by the depth symbol (↧) and the depth value. Example: ø10.0 ↧25.0 means a blind hole 10mm in diameter and 25mm deep. For threaded blind holes, the drill depth and thread depth are called out separately using thread notation.
The drill depth for a tapped blind hole should equal the required thread depth plus at least 1.5 times the thread diameter for chip clearance, plus the tap lead length. As a practical guideline, thread depth should not exceed 2x the thread diameter. Deeper thread engagement adds minimal strength while significantly increasing tap breakage risk.
The most frequent issues are chip packing at the bottom (leading to tool breakage), thermal buildup in hard materials like stainless steel or titanium, insufficient drill depth below threads causing tap breakage, and fluid entrapment during assembly. Peck drilling, pressure-fed coolant, and correct drill depth specification resolve most of these.
For standard CNC machining with conventional twist drills, the practical maximum is 3:1. Depths between 3:1 and 10:1 are possible with extended-reach drills, gun drills, or BTA deep hole drilling processes, but require specialist tooling and add cost. Designs exceeding 10:1 typically require redesign or splitting the feature across two operations.
No. The tip geometry of most taps means the last few threads at the very bottom of the hole will be partially formed. A bottoming tap reduces this runout zone to roughly 1-1.5 thread pitches, but it cannot achieve full thread engagement to the absolute bottom of the hole. If full thread engagement at the bottom is required, the design should be reconsidered or a flat-bottom drilled and bored extension used.
Blind holes are not difficult to manufacture when the drawing is clear. The problems usually start when the supplier has to infer the depth, thread length, bottom shape, or inspection requirement.
So the rule is simple: do not just mark the hole diameter. Specify the full feature.
For most CNC blind holes, that means calling out:
The more precise the callout, the easier it is for a CNC supplier to quote accurately, choose the right tooling, and machine the part without delays.
If your part includes blind holes, tapped holes, sealing features, or tight-tolerance drilling, you can submit your sourcing inquiry on Haizol and get quotes from verified CNC machining suppliers within 24 hours.