CNC Hole
Undersize:
Causes,
Diagnosis &
Solutions
Why are CNC holes undersize? Understand how tool wear, deflection, runout, thermal effects, material behaviour, cutting conditions, machining strategy and inspection can affect hole diameter.
A practical engineering guide for machinists, manufacturing engineers, design engineers, quality teams and manufacturing buyers. Diagnose the mechanism — not just the dimension.
↓
DIAGNOSE
↓
CORRECT
A CNC hole that finishes undersize is not necessarily caused by a drill that is simply “too small.” The finished diameter is the result of the complete machining system: tool geometry, tool condition, runout, machine behaviour, workholding, material, cutting forces, thermal conditions, chip evacuation, machining strategy and measurement.
Quick Engineering Answer
Confirm the Measurement
Verify the drawing, tolerance, gauge, cleanliness, measurement location and temperature.
Identify the Pattern
Determine whether the hole is consistently small, drifting, depth-dependent or randomly varying.
Correct the Mechanism
Fix wear, deflection, thermal drift, toolholding, chip evacuation or process selection.
Engineering principle: Do not immediately compensate for an undersized hole. First determine whether the process is stable and identify whether the problem is caused by tooling, process capability, machine behaviour or inspection.
What Does CNC Hole Undersize Actually Mean?
“Undersize” only has meaning relative to the drawing requirement. For example, a hole specified as Ø10.00 ±0.02 mm has an acceptable range of 9.98 to 10.02 mm.
A measured hole of 9.97 mm is therefore out of tolerance. But 9.97 mm could be acceptable for a different drawing with a lower limit below 9.97 mm.
| Observed Condition | What It May Suggest |
|---|---|
| Consistently undersize from the first part | Tool diameter, geometry, compensation, setup or process-selection issue. |
| Progressively smaller with production | Tool wear, thermal drift or another changing process condition. |
| Random variation between parts | Process instability, workholding, temperature, tooling or measurement variation. |
| Smaller deeper in the hole | Taper, deflection, chip evacuation, alignment or tool-condition issue. |
| Correct after reaming | Drilling may not have been capable of producing the required final bore. |
| Diameter correct but position wrong | Likely a datum, workholding, probing or coordinate-system issue. |
Measure Before You Change the Process
One of the most common troubleshooting mistakes is changing an offset before confirming that the measurement itself is valid. For a precision internal feature, the inspection method should match the tolerance and geometry.
Measurement Checklist
- Confirm the current drawing revision.
- Confirm nominal diameter and tolerance.
- Clean chips and coolant from the bore.
- Remove relevant burrs where they can influence measurement.
- Verify gauge condition and calibration.
- Repeat the measurement.
- Measure multiple depths when taper may exist.
- Consider part and gauge temperature for tight tolerances.
| Requirement | Potential Inspection Method | Purpose |
|---|---|---|
| General internal diameter | Suitable internal measurement | Direct diameter verification. |
| Precision bore | Bore gauge / internal micrometer | Controlled internal-diameter measurement. |
| Production GO / NO-GO requirement | Appropriate plug gauges | Fast functional acceptance. |
| Taper through depth | Bore gauge at multiple depths | Shows variation through the bore. |
| Position relative to datums | CMM or coordinate measurement | Diameter alone does not establish position. |
Main Causes of CNC Hole Undersize
Before changing tooling or offsets, classify the problem. The following cause families cover the most important engineering investigations.
| Cause Family | Typical Signature | First Investigation |
|---|---|---|
| Tool wear | Progressive dimensional drift. | Compare diameter against tool usage. |
| Built-up edge | Intermittent size and finish changes. | Inspect the cutting edge for adhered material. |
| Thermal effects | Size changes with machine or part temperature. | Compare dimension against production time. |
| Tool deflection | Depth-dependent or unstable geometry. | Review tool projection and cutting load. |
| Runout / toolholding | Geometry variation or unstable cutting. | Measure runout near the cutting end. |
| Tool geometry | Repeatable but abnormal result. | Inspect tool specification and cutting edges. |
| Chip evacuation | Deep-hole instability and heat. | Inspect flute packing and coolant delivery. |
| Material behaviour | Material-specific size variation. | Review grade, hardness and work hardening. |
| Process choice | Drilling cannot reliably hold required tolerance. | Evaluate reaming, boring or interpolation. |
| Inspection error | Different gauges give different results. | Cross-check the measurement method. |
Tool Wear
Tool wear is one of the most important causes of dimensional drift in repetitive hole production. The useful diagnostic question is not simply: “Is the tool worn?” It is: “Does hole diameter change predictably with tool usage?”
For example: 10.01 → 10.00 → 9.99 → 9.97 mm is a much more useful process signal than one isolated measurement.
Do not compensate indefinitely. Repeated offset corrections can move the dimension temporarily while the underlying tool deterioration continues.
What to Inspect
- Cutting-edge wear
- Margin condition
- Tool diameter
- Built-up material
- Tool usage count
- Coolant delivery
- Cutting severity
Built-Up Edge and Material Adhesion
Some work materials can adhere to the cutting edge under particular combinations of speed, feed, temperature, lubrication and tool geometry.
This changes the effective cutting geometry and can cause dimensional instability, poor finish and inconsistent hole size.
Inspect the cutting edge rather than assuming that the programmed tool diameter represents the actual cutting condition.
Depending on the material and tooling system, corrective actions can include reviewing cutting speed, feed, coolant/lubrication, tool geometry and tool condition.
Thermal Effects
A CNC machining process is not dimensionally static. Spindle heat, cutting heat, coolant temperature, machine warm-up and workpiece temperature can all affect a precision machining process.
Useful diagnostic: If hole size correlates strongly with time or thermal state, investigate thermal behaviour before blaming tool wear alone.
Record measurements at the beginning, middle and end of production and compare them against machine warm-up and production conditions.
Tool Deflection and Rigidity
Cutting tools deflect under machining forces. The effect becomes increasingly important with long tool projection, small tool diameter, deep holes, high cutting load and weak workholding.
| Condition | Why It Matters | Possible Response |
|---|---|---|
| Long tool projection | Lower bending stiffness. | Reduce projection where the geometry permits. |
| Small tool diameter | Lower bending stiffness. | Use the stiffest practical tooling. |
| Deep hole | Greater cutting and evacuation challenge. | Review tooling and drilling strategy. |
| High cutting load | Greater deflection. | Review cutting conditions and rigidity. |
| Weak workholding | Part movement or deformation. | Improve support and clamping. |
Runout and Toolholding
Tool runout should be investigated as part of the complete spindle–holder–tool system.
- Spindle interface
- Collet or chuck
- Tool shank
- Holder condition
- Seating surfaces
- Contamination
- Tool projection
Important distinction: Runout is frequently associated with oversized holes, unequal flute loading and poor hole geometry. It should not automatically be stated as a direct cause of every undersized hole. The actual error pattern must be investigated.
Incorrect Tool Geometry
Tool diameter alone does not define drilling performance. Point geometry, web thickness, helix, margins, coating, edge preparation and tool design can influence cutting forces, chip formation, wear and dimensional stability.
Tool selection should consider: Material + hole depth + tolerance + machine rigidity + coolant strategy + production volume.
Chip Evacuation
Chip evacuation becomes increasingly important as hole depth increases. Poor chip removal can result in recutting, friction, heat generation, flute packing and cutting-edge damage.
- Inspect chip shape and flute packing.
- Confirm coolant reaches the cutting zone.
- Review the hole depth-to-diameter relationship.
- Review pecking or chip-breaking strategy where applicable.
- Confirm the drill geometry suits the material.
Material Behaviour
The same nominal drilling process can behave differently in aluminium, stainless steel, alloy steel, titanium, engineering plastics and other materials.
| Material Behaviour | Potential Effect |
|---|---|
| High hardness | Higher cutting forces and increased tool wear. |
| Work hardening | Rubbing can make subsequent cutting more difficult. |
| Low thermal conductivity | Greater local heat concentration. |
| Adhesive behaviour | Built-up edge and unstable cutting geometry. |
| Elastic recovery | The finished feature can respond differently after the tool passes. |
| Thermal expansion | Measurement and actual part size can shift with temperature. |
Drilling vs Reaming vs Boring vs Interpolation
One of the most important engineering decisions is whether drilling should actually be the final diameter-generating operation.
The better question is: Can the selected process reliably achieve the required bore?
| Method | Main Strength | Typical Use | Key Consideration |
|---|---|---|---|
| Drilling | Fast hole generation. | General-purpose holes. | May not suit demanding final bore tolerance. |
| Reaming | Controlled finishing. | Improved size consistency and finish. | Requires suitable pre-hole and allowance. |
| Boring | Adjustable diameter control. | Precision bores and larger holes. | Potentially higher cycle time. |
| Circular interpolation | Flexible CNC diameter generation. | Certain precision and flexible-production applications. | Toolpath, machine and tool capability matter. |
For demanding hole requirements, a controlled finishing operation can be more robust than repeatedly changing a drilling offset.
Cutting Parameters
Cutting parameters are application-specific. Actual values should come from the tooling manufacturer and be adapted to the machine, material, coolant and rigidity.
n
= spindle speed (rpm)
Vc
= cutting speed (m/min)
D
= tool diameter (mm)
Example: If a hypothetical tool/material combination calls for Vc = 100 m/min with a 10 mm tool , the calculated spindle speed is approximately 3183 rpm.
Vf
= feed rate (mm/min)
n
= spindle speed (rpm)
fn
= feed per revolution (mm/rev)
Example: At 3000 rpm and 0.10 mm/rev, Vf = 300 mm/min. This is an illustrative calculation, not a universal machining recommendation.
Step-by-Step Diagnosis Workflow
Hole Tolerance, Depth and Process Capability
Hole tolerance should be treated as a functional requirement, not simply a number entered into CAD. Tighter tolerances can change the required tooling, process sequence, inspection method, process control and production cost.
| Design Question | Why It Matters |
|---|---|
| Is the tolerance functionally necessary? | Tighter tolerances increase process and inspection demands. |
| Is the hole deep relative to diameter? | Deflection and chip evacuation become more challenging. |
| Can a standard drill diameter be used? | Standard tooling generally simplifies process planning. |
| Does the bore need controlled finish or geometry? | A dedicated finishing operation may be more appropriate. |
| Can the feature be inspected reliably? | Manufacturability includes practical verification. |
Continue with the CNC Hole & Thread Design Guide , CNC Machining Tolerances and High-Precision CNC Design Rules .
Practical CNC Hole Undersize Examples
Example 1 — Progressive Diameter Drift
A Ø12.00 ±0.03 mm hole begins at 12.01 mm and gradually moves toward 11.96 mm during production. The first investigation should compare hole size against tool usage and machine thermal state.
Example 2 — Hole Becomes Smaller With Depth
A nominal 10 mm hole measures: 9.99 mm at entry, 9.97 mm in the middle, 9.95 mm deeper inside. This pattern should trigger investigation of taper, deflection, chip evacuation, alignment and tool condition.
Example 3 — Precision Finishing Requirement
A drawing calls for Ø20.000 ±0.010 mm while drilling repeatedly produces variable results. Instead of repeatedly changing offsets, evaluate whether reaming, boring or interpolation is a more appropriate finishing strategy.
Production and Cost Impact
An undersized hole can lead to scrap, rework, additional inspection, tool replacement, machine downtime, sorting, customer rejection and delivery delays.
The best solution is therefore not necessarily the theoretically fastest cycle. The objective is a process that produces the required feature reliably and economically.
For related manufacturing economics, see: CNC Machining Cost and Reduce CNC Machining Cost .
CNC Hole Undersize Checklist
Before Machining
- ☐ Drawing revision confirmed
- ☐ Hole nominal and tolerance confirmed
- ☐ Material and grade confirmed
- ☐ Hole depth checked
- ☐ Position and GD&T checked
- ☐ Drilling vs finishing process evaluated
- ☐ Tool diameter verified
- ☐ Tool geometry verified
- ☐ Tool projection minimized
- ☐ Holder / collet clean
- ☐ Workholding verified
- ☐ Coolant delivery verified
When the Hole Is Undersize
- ☐ Recheck measurement
- ☐ Check tool wear
- ☐ Inspect cutting edge
- ☐ Check runout
- ☐ Check toolholder
- ☐ Check chip evacuation
- ☐ Review cutting conditions
- ☐ Check thermal behaviour
- ☐ Check material condition
- ☐ Check compensation
- ☐ Evaluate finishing operation
Frequently Asked Questions
Why is my CNC-drilled hole smaller than the drill diameter?
A drill does not necessarily reproduce its nominal diameter perfectly. Tool condition, geometry, runout, cutting forces, material response, thermal effects, chip evacuation and measurement can all influence the finished hole.
Can a worn drill make a hole undersize?
Yes. Tool deterioration can change cutting behaviour and produce dimensional drift. A progressive relationship between hole size and tool usage is especially useful evidence.
Should I simply increase the tool offset?
Only after confirming that the process is stable and the error is consistent. Compensation should not be used to hide an unstable tool, thermal drift, runout or another underlying problem.
Why is the hole correct at the top but smaller deeper down?
Possible causes include taper, tool deflection, tool condition, chip evacuation, coolant access and alignment. Measure the bore at multiple depths before changing the process.
When should I ream instead of drill?
Consider reaming when the required size consistency and surface finish exceed what the drilling process can reliably provide. The pre-hole must be appropriate for the reaming operation.
Can material temperature affect hole size?
Yes. Thermal expansion can influence both the workpiece and the measurement system.
Why can the same drill produce different hole sizes on two CNC machines?
Machine rigidity, spindle condition, toolholding, coolant, workholding, material condition and cutting conditions can differ. The drill is only one part of the machining system.
Does CNC machine positioning accuracy guarantee accurate holes?
No. Positioning accuracy is only one part of hole quality. Tool geometry, deflection, runout, workholding, material behaviour and inspection also affect the result.
Related CNC Engineering Resources
A hole-size problem often connects to broader questions about tolerances, tooling, inspection, dimensional stability and machining strategy.
CNC Dimensional Inaccuracy
Diagnose dimensional errors caused by tooling, WCS, workholding, thermal behaviour and inspection.
CNC Hole & Thread Design Guide
Design considerations for holes, threads, depths and manufacturability.
CNC Machining Tolerances
Understand tolerance selection, precision and manufacturing implications.
CNC Cutting Tools
Explore tool types, selection and CNC machining applications.
CNC Spindle Runout
Understand runout and its relationship to machining precision.
CNC Tool Wear
Understand tool wear mechanisms and dimensional effects.
CNC Inspection
Match inspection methods to machining requirements.
CNC Machining Limitations
Understand feature depth, tooling, access and process limitations.
Recommended Visuals for This Knowledge Hub Page
Hole Undersize Diagnostic Tree
Measurement → error pattern → tool → machine → material → process → verification.
Bore Measurement at Multiple Depths
Show entry, middle and bottom measurements to reveal taper or depth-related variation.
Drill vs Ream vs Bore
Explain why different hole-making processes are selected for different tolerance requirements.
Tool Wear vs Hole Diameter
Plot measured diameter against tool usage to illustrate progressive process drift.
Have a CNC Drawing With a Difficult Hole?
Use this guide to understand the likely machining mechanism first. When the requirement involves difficult tolerances, unusual materials, complex geometry or production scaling, an engineering review can help evaluate process selection, manufacturability and inspection.
Discuss a Manufacturing Requirement