Dimensional Error — Why Your Part Is the Wrong Size
The tool looks right, the program looks right, but the dimension is off. Dimensional errors are frustrating because the cause is rarely obvious — it could be tool wear, thermal growth, deflection, backlash, or a bad setup. This page helps you diagnose and fix the most common causes.
The Diagnostic Approach
Before adjusting anything, ask: is the error consistent or random?
| Pattern | Suggests |
|---|---|
| Same error every part, same direction | Offset error — tool offset, work offset, or setup |
| Error grows as batch progresses | Tool wear or thermal growth |
| Error varies between parts randomly | Setup inconsistency, chips under part, loose vise |
| One direction OK, other direction off | Backlash or axis-related error |
| Part is tapered (one end bigger/smaller) | Deflection or misalignment |
1. Taper (Part Not Parallel)
A bored hole or turned shaft that's larger at one end than the other.
| Cause | How to identify | Fix |
|---|---|---|
| Tool deflection (boring bar flex) | Taper is consistent, larger at the free end | Stiffer boring bar (larger diameter, shorter), reduce feed |
| Z-axis not aligned to spindle | Taper direction flips if you reverse the part | Machine alignment issue — call maintenance |
| Workpiece deflection | Part flexes under cut, springs back | Support better, reduce DOC, use climb milling |
| Tool wear over long cut | Taper increases with cut length | Sharper tool, peck cycle, shorter cut |
2. Dimensional Drift Over Time
Parts start in tolerance, but after running for an hour, dimensions drift.
Thermal Growth
The spindle and machine heat up during the day, expanding. A 500 mm steel spindle can grow 0.03–0.05 mm after warm-up. The part also heats up.
Typical pattern: first part of the morning is slightly small; by lunch it's slightly large; by end of day it's drifted 0.02–0.05 mm.
Fix:
- Warm up the machine for 15–20 minutes before precision work (run the spindle at operating speed).
- Let parts cool to room temperature before measuring.
- Use in-process offsets — measure every N parts and adjust the offset.
- For critical parts, measure the part temperature and apply compensation.
Tool Wear
As the tool wears, it cuts smaller (for an external cut) or larger (for an internal bore). The error grows linearly with cutting time.
Fix: track tool life by number of parts or cutting time. Replace the tool before it drifts out of tolerance. For production, use tool wear offset adjustments in the program.
3. Backlash
When the axis reverses direction, there's a small gap between the screw and nut — the axis doesn't move for a small distance. This shows up as position error on features machined from opposite directions.
| Symptom | When it happens |
|---|---|
| Hole position offset when approaching from opposite sides | Boring cycles, pocket milling that reverses direction |
| Linear dimensions OK, but stepped features are off | Axis reverses between steps |
Fix: most modern CNCs have backlash compensation in parameters. If backlash is excessive, the ballscrew may need adjustment or replacement.
4. Workpiece Deflection
The part flexes under cutting force, then springs back when the tool leaves. This makes thin walls too thin or pockets too shallow.
| Symptom | Fix |
|---|---|
| Thin walls thinner at the middle | Climb mill, lighter cuts, support from behind |
| Pocket floor not flat (bowed) | Reduce DOC, use stiffer tool, leave finish stock |
| Part moves in the vise during cut | Tighten setup, use soft jaws, support better |
5. Setup and Offset Errors
These are operator errors — the machine is fine, but the setup is wrong.
| Mistake | Symptom | Fix |
|---|---|---|
| Work offset (G54) set wrong | All features offset by the same amount | Re-edge-find or re-touch off the part |
| Tool length offset wrong | Z dimensions all off (depth, pocket floor) | Re-check tool length setting |
| Tool diameter offset wrong | Milled pockets are consistently too big/small | Calibrate tool diameter probe or measure |
| Chips under the part | Z dimension off by a small random amount | Clean parallels and part before setup |
| Part not seated flat | Angular error, inconsistent dimensions | Tap down, check with indicator |
6. Poor Surface Finish (Non-Chatter Causes)
Not all bad finish is chatter. Common causes:
| Cause | What it looks like | Fix |
|---|---|---|
| Dull tool | Torn, smeared surface | Index or replace |
| BUE | Gummy, built-up appearance | Increase speed (see Tool Wear) |
| Feed too high | Deep feed marks | Reduce feed, larger nose radius |
| Wrong coolant | Built-up edge, heat marks | Use correct coolant, increase flow |
| Built-up edge breaking off | Random scratches/digs in surface | Increase speed, use coated tool |
Systematic Troubleshooting Procedure
- Measure the error: record which dimension is off, by how much, in which direction.
- Check the pattern: consistent? growing? random? one axis?
- Verify the basics: is the tool sharp? Is the offset correct? Is the part clean and seated?
- Warm up: run the machine 15 min, re-measure. If error changes, it's thermal.
- Check tool wear: inspect the edge under magnification.
- Test one variable at a time: change speed, then feed, then setup — don't change everything at once.
- Document the fix: note what worked on the setup sheet for next time.
Remember: when in doubt, measure first. Don't adjust an offset based on a single bad part — measure two or three to confirm the pattern. One bad reading could be a chip under the part or a measurement error.