Blind Hole vs Through Hole: Definitions, Drawing Symbols, and Design Rules
Thru holes exit the part; blind holes stop inside it. That one geometric difference drives chip evacuation, coolant delivery, depth control, bottom shape, tapping strategy — and cost. Here is how to call out each correctly and choose between them.
IsoCNC Engineering Team
CNC Machining & DFM Engineers · Updated · 15 min read
On this page
Quick Answer
A through hole passes completely through the workpiece and opens on two faces; a blind hole stops at a specified depth inside the material. On drawings, thru holes are called out with the diameter plus THRU, while blind holes use the depth symbol ↧ followed by a depth value (⌀10 ↧ 25) that applies to the full-diameter portion only. Through holes are easier and cheaper to machine — chips and coolant flow straight through, no depth stop is needed, and tapping runs in one pass. Blind holes are mandatory when the far face must stay sealed, clean, or structurally intact, but they demand peck drilling, careful depth measurement, and bottoming taps.
What Each Term Means — and How Drawings Call Them Out
A through hole (thru hole) breaks out the far side of the part; a blind hole terminates at a controlled depth inside it. Every other machined feature — counterbores, countersinks, spotfaces — is a variation on one of these two primitives. A counterbore is really a shallow, large-diameter blind hole coaxial with a smaller hole, and a countersink is its conical cousin; both are covered in our guide to countersink and counterbore holes.
The drawing callouts differ in one keyword. A through hole is written as the diameter plus THRU: ⌀10 THRU. A blind hole carries the depth symbol ↧ (Unicode U+21A7, a downward arrow) before the depth value: ⌀10 ↧ 25 means a 10 mm hole, 25 mm deep. The convention that saves arguments later: the depth value describes the full-diameter cylindrical portion of the hole. The conical drill point below that shoulder is extra stock the shop adds automatically, and it is not counted in the ↧ figure. If your design genuinely needs 25 mm of usable cylinder plus knows the point exists below it, the standard callout already says exactly that.
Threaded holes follow the same logic. A blind tapped hole callout should state the thread size and the full thread depth — for example M8 × 1.25 ↧ 16 — and, where depth is tight, a separate drill depth note so the machinist knows how much non-threaded allowance exists below the last full thread. Ambiguity here is the single most common cause of undersized thread engagement we see on incoming prints.
Why Blind Holes Fight Back: Chips, Coolant, and Depth
A through hole is the friendliest feature in machining: chips ride the coolant stream out the far side, the drill never has to stop on a position, and gauges pass straight through. A blind hole closes that exit, and three problems arrive together. Chip evacuation turns around — every chip must travel back up the flutes against the incoming coolant. Past roughly three diameters of depth, shops switch to peck drilling cycles that retract the drill to clear chips; past five diameters, through-tool coolant stops being a luxury. Coolant delivery degrades for the same reason, which heats the cutting edge and shortens tool life. And depth control becomes a real operation: the machine must stop the drill at a programmed Z position, and someone must verify it afterward.
That verification is its own cost center. A through hole is checked with calipers, pin gauges, or a bore gauge passed straight through. A blind hole’s depth is measured indirectly with a depth micrometer, a vernier depth gauge, or a touch probe, and the condition of the bottom — clean or packed with chips — is invisible without a borescope. Deep holes multiply all of it: industry guidance treats anything past about 10:1 depth-to-diameter as deep-hole territory requiring through-coolant tooling, and gundrilling beyond that. For how these process limits interact with the numbers on your print, see our reference on CNC machining tolerances. And features a drill or end mill cannot form at all — deep square pockets, narrow slots in hardened steel — are typically cut by wire EDM instead.
| Factor | Through Hole | Blind Hole |
|---|---|---|
| Chip evacuation | Chips exit through the far side with the coolant stream | Chips must travel back up the flutes against the inflow; peck cycles needed past ~3×D |
| Coolant delivery | Flood coolant reaches the cutting edge and flushes through | Coolant fights rising chips; through-tool coolant strongly recommended past ~5×D |
| Depth control | Breakthrough is self-limiting — no depth stop required | Z-depth must be programmed and held; bottom position verified after machining |
| Bottom form | Exit burr only; deburr the far face | Conical drill-point residue (118°–135°) unless finished flat with an end mill |
| Measurement | Calipers, pin gauges, and bore gauges pass straight through | Depth checked indirectly with a depth micrometer or probe; bottom unseen without a borescope |
| Tapping | Spiral-point taps push chips ahead; full thread to the exit face | Spiral-flute taps plus a bottoming chamfer; drill 3–5 pitches past the thread |
| Relative cost | Baseline — fastest to make, inspect, and deburr | Adds peck cycles, tool changes, and inspection steps; budget a premium |
Bottom Geometry: The Drill Point You Did Not Draw
A standard twist drill has a point angle between 118° and 135°, so every drilled blind hole ends in a cone. This is not a defect and not optional — it is the shape of the tool. The drawing convention handles it: the ↧ depth applies to the full-diameter portion, and the shop drills deeper to put the cone below it. Problems start only when a designer forgets the cone exists. A fastener stack calculated to the nominal depth, a pin pressed to the bottom, or a part sectioned too thin behind the hole can all collide with drill point residue that was never on the print but was always going to be there.
When the floor genuinely must be flat — a spring seat, a magnet pocket, a controlled clearance under an insert — the hole gets a second operation. A flat-bottom drill can convert the cone in one pass, and an end mill plunged into the drilled hole produces a true flat floor with a small corner radius at the wall. Either way you have added a tool change, a setup consideration, and an inspection note. Specify flat bottoms only where function requires them, and call the requirement out explicitly: a note like ⌀12 ↧ 20 FLAT BOTTOM removes all ambiguity. If the floor is merely cosmetic or clearance, accept the standard conical bottom and save the money.
Tapping Blind Holes: Bottoming Taps, Drill Margin, and Thread Relief
Blind hole tapping is where good drawings go to die. A tap cannot cut full thread to the very bottom of a hole, because the chamfered lead threads at its tip are incomplete by design. How incomplete depends on the tap style — and choosing the right one is the whole game.
| Tap Style | Chamfer Length | Best Use |
|---|---|---|
| Taper tap | 7–10 threads | Easy starting and hand tapping; cannot thread anywhere near a hole bottom |
| Plug tap | 3–5 threads | General-purpose CNC tapping; the standard choice for through holes and roomy blind holes |
| Bottoming tap | 1–2 threads | Blind holes that need full thread close to the floor; follow a plug tap for tool life |
Two process rules follow. First, use a spiral-flute tap in blind holes: its helical flutes pull chips up and out, the reverse of a spiral-point (gun) tap, which pushes chips ahead and is the right tool only for thru holes where the chips have somewhere to go. Second, drill deeper than the thread — the standard allowance is three to five thread pitches beyond the full thread depth, so the tap’s chamfer and the chip load never meet the bottom. An M8 × 1.25 hole needing 16 mm of full thread wants roughly 20–22 mm of drill depth. When the part cannot spare that, a thread relief groove at the bottom of the threaded section gives the tap somewhere to end. Our tapped hole design guide covers thread engagement, drill sizes, and callout formats in full.
Broken taps are the expensive version of getting this wrong. A tap that bottoms on packed chips or the drill cone snaps, and removing a hardened tap fragment from a blind hole in a nearly finished part can cost more than the part itself. Generous drill margin, the right tap geometry, and rigid tapping cycles with peck retracts are cheap insurance.
When a Blind Hole Is the Only Choice
Given the cost gap, blind holes should earn their place. They do in four situations. Sealing: the far face is a pressure or fluid boundary — hydraulic manifolds, pneumatic blocks, coolant passages — where a breakthrough would leak or need a plug. Cosmetics: the far face is a visible Class-A surface that a drill exit burr or a plug would spoil, common on enclosures and consumer-facing panels. Fastener containment: a screw or dowel must not protrude beyond the part — either because something moves behind it, or because the assembly stacks flush. Structure: the material behind the hole is load-bearing or intersects other features, and removing it would weaken the part or collide with a crossing bore.
If none of those apply, challenge the blind hole on the print. A remarkable share of them are simply the CAD default — the designer sketched a hole to a depth, and nobody asked whether it could go through. Thick sections can also be drilled from both sides as two opposed thru holes, meeting in the middle; the small mismatch at the junction is usually acceptable and much cheaper than a single deep blind hole. When a blind hole is mandatory, help the shop: keep depth under five diameters where possible, use standard drill sizes, allow the full drill-point allowance, and state the full thread depth separately from the drill depth.
The Cost Case for Through Holes — and a DFM Checklist
Every disadvantage in the table above is a line item. A thru hole drills in one continuous pass, deburrs on the exit face, reams or bores with through-access tooling, taps in a single pass with a spiral-point tap, and inspects with gauges that pass through it. A blind hole adds peck cycles, a programmed depth stop, a bottom-cleaning consideration, possible flat-bottom tooling, a bottoming tap operation, and indirect inspection. On a quote, a deep or threaded blind hole routinely costs several times what the same diameter thru hole costs. The cheapest hole is the one that goes through.
Before releasing a drawing, run this checklist on every hole. Can it go through without breaking a seal, a cosmetic face, or a mating surface? If it must be blind, is the depth under five diameters — and if not, can it be drilled from both sides? Is the diameter a standard drill size? Does the callout use ↧ with the depth to the full-diameter portion, leaving room for the drill point? For tapped blind holes, is the drill depth three to five pitches beyond the full thread depth, or is there a thread relief? And does any flat-bottom requirement carry an explicit note? These are exactly the questions in our broader DFM guide for CNC design — answer them on the print and the quote comes back shorter, cheaper, and with fewer questions.
FAQ: Blind Holes vs Through Holes
What is the difference between a blind hole and a through hole?
A through hole passes completely through the workpiece and opens on two faces; a blind hole stops inside the material and opens on one face only. On a drawing, a through hole is called out with the diameter plus THRU, while a blind hole carries the depth symbol ↧ followed by a depth value — for example ⌀10 ↧ 25. The distinction matters because everything downstream changes: chip evacuation, coolant delivery, depth control, bottom geometry, and tapping strategy all get harder when the hole has a floor instead of an exit, and each of those shows up in the piece price.
How do you show a blind hole on an engineering drawing?
Use the diameter symbol, the hole size, the depth symbol ↧, and the depth: ⌀10 ↧ 25 means a 10 mm hole, 25 mm deep. By convention the depth value refers to the full-diameter cylindrical portion — the conical drill point below it is extra and not counted. A through hole replaces the depth with the note THRU, as in ⌀10 THRU. For threaded blind holes, call out the full thread depth and, when space is tight, the drill depth separately so the shop knows exactly how much non-threaded allowance it has to work with.
Why are blind holes harder to machine than through holes?
Three mechanisms stack up. Chips have nowhere to go but back up the flutes against the incoming coolant, so blind holes deeper than about three diameters need peck cycles or through-tool coolant to avoid packing and drill breakage. Coolant delivery to the cutting edge is worse for the same reason, which shortens tool life. And the hole must stop at a controlled Z position that is verified afterward with a depth micrometer or probe, since nothing can pass through to check it. Each item adds cycle time, tool wear, and inspection cost.
How do you tap a blind hole correctly?
Drill deeper than the required thread — a margin of three to five thread pitches is the common shop rule — so the tap never bottoms on chips or the drill cone. Use a spiral-flute tap, which pulls chips up and out of the hole, and finish with a bottoming tap (a chamfer of only one to two threads) when full threads must run close to the floor. If the design cannot spare the extra drill depth, add a thread relief groove at the bottom of the threaded section. Always call out the full thread depth on the drawing so the shop can plan the allowance.
Can a blind hole have a flat bottom?
Yes, but not from a standard twist drill. A normal 118°–135° drill point leaves a conical floor, and the drawing depth applies only to the full-diameter portion above it. If the floor must be flat — for a spring seat, a magnet pocket, or a controlled clearance — the hole is finished with a flat-bottom drill or plunged with an end mill after the twist drill. That adds a tool change and cycle time, so specify flat bottoms only where the function genuinely requires them, and note the requirement explicitly on the drawing rather than assuming the shop will infer it.
When should I use a through hole instead of a blind hole?
Whenever the design allows it. Through holes are cheaper at every step: chips exit freely, coolant flushes the cut, no depth stop or bottom inspection is needed, reaming and boring tools can pass through, and spiral-point taps thread them in a single pass. Convert a blind hole to a through hole unless the far face must stay sealed against pressure or fluid, must remain cosmetically clean, or must keep a mating screw from protruding. If a blind hole is truly mandatory, keep it shallow, keep the diameter generous, and be explicit about the full thread depth.
Designing holes that must be drilled, tapped, and gauged? The CNC machining services page covers the processes involved, and China CNC machining
Related Resources
CNC Machining Surface Finish: The Ra Chart, Explained
The CNC machining surface finish chart: Ra values in μm and μin, N1–N12 grades, what each process achieves, what…
Passivation of Stainless Steel: Process, Specs, and When Parts Need It
Passivation of stainless steel explained for machined parts: the chemistry, ASTM A967 and AMS 2700 methods, nitric…
GD&T Basics for CNC Machined Parts: The Symbols That Matter
GD&T basics for machined parts: the 14 symbols explained, feature control frames, datums, MMC bonus tolerance, true…
How to Outsource CNC Machining to China, Step by Step
How to outsource CNC machining to China, step by step: vet suppliers, compare landed cost, control quality remotely,…
Holes on Your Print? Send the Drawing.
IsoCNC machines blind and thru holes, tapped holes, counterbores, and deep-hole features in aluminum, steels, stainless, titanium, and brass — with thread gauges, depth verification, and full inspection reports on every lot. An engineer reviews every RFQ, typically within 1–2 business days.