A blind hole looks simple on a drawing: it stops before breaking through the workpiece. In practice, that closed bottom changes how the hole is machined. Chips must come back out through the entry, the tool needs room to finish cutting, and a tapped hole needs clearance below the complete threads.
Start by deciding which surface does the real work. A depth callout might mean total drilled depth, full-diameter usable depth, or complete thread depth. Once that is clear, the machining and inspection plan becomes much easier to build.
Blind Holes and Through Holes are not the same
A through hole gives chips and coolant another way out. A blind hole does not. The closed end may be needed for appearance, sealing, assembly, or another design reason. It also makes chip control and depth inspection more demanding.
Use a blind hole when that closed end has a clear job. If a through hole works just as well, it often gives the tool, chips, and inspector better access.
Define Blind Hole Depth before Choosing a Tool
The word “depth” can refer to several different surfaces. A useful drawing names the surface or cylindrical zone that must meet the requirement.
Total drilled depth and usable full-diameter depth
A standard twist drill leaves a conical point at the bottom. Total drilled depth reaches the tip of that cone. Usable depth stops where the straight, full-diameter wall ends.
Those two dimensions are easy to confuse, but they do not describe the same feature. If a pin, insert, fastener, or fluid passage needs a cylindrical zone, call out the usable depth. The process plan can then include the drill-point allowance and any clearance required by the chosen tool.
Avoid copying a standard allowance from another drawing. The needed distance changes with drill-point geometry, diameter, material, breakthrough risk, and the inspection method.
Conical and flat-bottom blind holes
A conical bottom is the normal result of twist drilling. In many parts, that is perfectly acceptable because the bottom shape has no functional role.
A flat bottom needs another tool or an additional operation. Depending on the diameter, depth, access, and finish, the process may use a flat-bottom drill, end mill, circular milling path, or boring operation. The drawing should still define the corner condition and usable depth. A note that says “flat” does not automatically require a perfectly sharp internal corner.
Drilled depth and complete thread depth
A blind tapped hole needs more drilled depth than complete thread depth. The lead section of the tap does not cut a complete thread. The process also needs space for chips and tool runout below the usable threads.
The screw adds one more limit. Its engaged length must not reach the bottom before the joint clamps. Review the screw length, mating-part thickness, washers, thread engagement, incomplete thread zone, and bottom clearance as one stack.
Match the Machining Method to the Result
Choose the operation by the feature you need to control. The methods below may start with the same hole, but they do different jobs.
| Method | Use it to control | Watch for | Verify |
|---|---|---|---|
| Drilling | Create the hole quickly and establish its axis and depth | Drill-point bottom, chip packing, runout, depth drift | Entry, depth, diameter, position |
| Circular or helical milling | Adjust diameter by toolpath and machine a controlled bottom profile when access permits | Tool deflection, interpolation error, corner condition | Diameter, roundness, bottom form, position |
| Boring | Enlarge and correct an existing hole’s diameter, alignment, or form | Bar clearance, vibration, bottom collision | Diameter, taper, roundness, bottom profile if specified |
| Reaming | Improve the size and finish of a prepared cylindrical wall | Reamer lead, stock allowance, trapped chips, insufficient bottom clearance | Finished diameter, taper, surface condition |
| Tapping | Cut an internal thread | Incomplete lead threads, chip evacuation, torque, bottom contact | Complete thread depth and functional thread acceptance |
| Thread milling | Produce a thread with a helical toolpath and adjustable size control | Cutter access, minimum hole size, tool reach, programming | Thread size, depth, position, entry and exit condition |
Boring can improve diameter and alignment, but it does not control blind-hole depth by itself. Reaming also does not create a sharp, flat bottom. Finishing tools still need clearance, and the bottom shape may require its own operation.
For a broader look at drill selection and cycle planning, see our guide to CNC drilling. A blind hole still needs a clear depth and bottom definition of its own.
Manage Chips, Heat, Deflection, and Depth
Chips have only one practical way out of a blind hole. If they collect under the cutting edge, torque and heat rise. The tool may rub, recut chips, mark the wall, or stop before reaching the programmed depth.
Good chip control starts with the material and tool geometry. Aluminum can produce long chips under some cutting conditions. Flute space, edge geometry, lubrication, coolant delivery, and the withdrawal strategy therefore need to work together.
A fixed peck cycle is not always the safest answer. Too many short retracts waste time and may let chips fall back into the cut. Too few can overload the flutes.
Set the cycle from the actual chip shape, hole depth, toolmaker guidance, and a stable trial. Coolant delivery must suit the tool and machine as well. Treat any published coolant recommendation as tool-specific guidance, not as a universal setting for every blind hole.
Depth control also depends on the reference surface and setup. Check tool length compensation, spindle growth, workholding movement, entry geometry, chip buildup, and the method used to touch or probe the surface. If depth is critical, confirm the first part and monitor the feature with the agreed inspection method.
Tapping a blind hole
The tap must either carry chips away from the closed end or keep them controlled in the space available. Gühring’s tapping guidance recommends right-hand spiral-flute taps for suitable blind-hole applications because they direct chips back up the flutes. The same guide shows that chamfer length affects the bottom clearance the tap needs.
Tap selection still depends on the thread form, material, hole diameter, pitch, coating, lubrication, machine synchronization, and chip behavior. Thread milling can help when adjustable thread size, chip control, or recovery from a broken tool matters. It still needs suitable machine motion, cutter access, and enough room for the tool.
Put the Important Details on the Drawing
A machinist should not have to guess which part of the hole performs the function. Name the required feature and the basis for accepting it.
Include these items when they affect the part:
- hole diameter and tolerance;
- total drilled depth or full-diameter usable depth;
- conical, flat, radiused, or otherwise controlled bottom form;
- thread specification and complete thread depth;
- position, orientation, datum references, and any geometric control;
- entry chamfer, spotface, counterbore, or edge-break requirement;
- remaining wall or breakthrough restriction;
- surface finish where it affects sealing, wear, or assembly;
- material, temper, quantity, and any coating or masking requirement;
- inspection or reporting requirement for a critical feature.
ASME Y14.5 provides rules for communicating dimensioning and tolerancing requirements. Use the standard and edition named by the project. A general shop note should not leave the functional depth or bottom surface open to interpretation.
Inspect the Feature that Matters
One gage cannot confirm every blind-hole requirement. Match the inspection method to the controlled feature and the access around it.
Depth may be checked with a suitable depth gage, probe, CMM strategy, or dedicated fixture. The contact point must reach the surface named on the drawing. A broad contact may bridge a conical bottom, while a narrow contact may reach the deepest point. Both readings can be correct, but they answer different questions.
Diameter checks also depend on how close the controlled zone sits to the bottom. Some standard internal gages need more approach distance than the feature allows. A purpose-built instrument, such as a Mitutoyo bore gage for blind holes, shows why near-bottom access belongs in the inspection plan.
Thread acceptance may use the specified functional gage, depth verification, or another method approved by the contract. Position and orientation need the stated datums. Our aluminum CNC machining tolerance guide explains how feature tolerances, datums, process planning, and inspection fit together.
Troubleshoot Common Blind-hole Problems
Start with the symptom, then change one likely cause at a time. A controlled first-part trial makes the real cause easier to find.
| Symptom | Likely mechanism | Check first | Corrective direction |
|---|---|---|---|
| Hole is too shallow | Chips under the tool, incorrect offset, tool wear, or setup movement | Bottom condition, tool length, reference surface | Clear chips safely, correct the offset, replace the tool, or stabilize the setup |
| Rough wall or smeared finish | Chip recutting, built-up edge, poor lubrication, or tool deflection | Chip shape, cutting edge, coolant delivery | Improve chip formation and evacuation, restore the edge, or reduce deflection |
| Taper or poor roundness | Runout, deflection, unstable workholding, or a finishing-tool problem | Tool runout, holder, setup, diameter by depth | Stabilize the tool and part, then finish with the method matched to the tolerance |
| Tap breakage | Packed chips, too little bottom clearance, alignment error, wear, or excess torque | Chip direction, drilled depth, tap lead, synchronization | Restore clearance and chip flow, correct alignment, or change the threading route |
| Screw bottoms before clamping | Fastener stack exceeds usable thread and clearance | Screw length, mating stack, complete thread depth | Shorten the screw, revise the stack, or increase qualified hole depth |
| Unintended breakthrough | Wrong depth reference, thin remaining wall, drill-tip allowance error, or part variation | Drawing basis, stock condition, actual wall | Correct the depth definition or redesign the feature with a safe remaining wall |
Use compressed air or flushing only when the machine, material, fluid, part geometry, and shop safety procedure allow it. A general cleaning instruction should not override the approved process.
Know When to Redesign the Feature
Sometimes a blind hole adds risk without adding value. If the exit is acceptable, a through hole may make chip removal and inspection much easier. A counterbore, pocket, access opening, insert, or revised joint can also reduce the required depth or threading difficulty.
Review the design carefully when the hole approaches a thin wall or needs a sharp, flat corner. The same applies when complete threads leave little bottom clearance or the required depth is difficult to inspect. Compare the functional need with the extra machining and inspection work before releasing the drawing.
What to Send for a Manufacturing Review
At Zheng Ji Aluminum, we review aluminum CNC drawings as part of the quotation process. For a blind hole, send the material and temper, 2D drawing or model, hole diameter, usable or threaded depth, bottom form, tolerance, inspection requirement, quantity, and surface treatment.
That information lets us review the feature in the context of the whole part. It also avoids the assumption that one tool, allowance, or inspection method works for every blind hole. You can review our aluminum CNC machining service or send us your drawing package with the blind-hole requirements marked clearly.
Blind Hole Machining FAQ
How much extra depth should be added below the usable part of a blind hole?
There is no universal allowance. The added depth must cover the selected drill-point geometry and any clearance needed by the finishing or threading tool. It must also preserve the required remaining wall. Put the usable depth on the drawing, then let the qualified process plan define the total depth.
What Tap Works Best for a Blind Hole?
A spiral-flute tap is a common choice for blind holes in long-chipping materials because it can carry chips back toward the entry. Short-chipping materials or another thread-making method may need a different tool. Choose the tap from the material, thread specification, available bottom clearance, machine, and lubrication plan.
Can a reamer make a flat-bottom blind hole?
Reaming controls the diameter and finish of a prepared cylindrical wall. A standard reamer has lead geometry and needs bottom clearance. It should not be the operation that defines a sharp, flat bottom. Machine the bottom with a suitable method, then ream the wall if the size and finish require it.
How is blind-hole depth inspected?
Use a method that contacts the surface named on the drawing. A conical drill tip, flat bottom, complete thread depth, and usable cylindrical depth are different features. Record which feature is measured, the datum or reference surface, and the approved instrument or program.
