Lesson 12.1: Clearance, Tap Drills, and the 0.15 mm Rule

---

Technical Context

This module collects dimensions and practices that the team can standardize instead of deciding again for every part.

Post these values in the build area and use them in CAD templates, drawings, and inspection checks.

---

The one rule behind all of it

A screw needs room to pass. The minimum clearance is 0.15 mm per side, so 0.3 mm on the diameter. Under that, the joint stops behaving like a clamped joint and starts behaving like a pin in a hole.

That number is not arbitrary. It has to absorb four things at once:

What it absorbs	Typical size
Drill cutting oversize or undersize	0.05 to 0.1 mm
Position error between two parts	0.1 mm or worse across a stack
Thread and head runout on the fastener	small, but real
Paint, anodising, burrs, and swarf	small, and always there

Add those and 0.3 mm on the diameter is the honest floor, not a generous allowance.

A hole cut exactly to the screw size is not a clearance hole

An M3 screw through a 3.0 mm hole binds. The parts cannot pull together, so tightening loads the screw in shear instead of clamping the faces, and the joint develops slop the first time it is hit. It also cannot be assembled without persuasion, which is how holes get reamed out with a drill bit at a competition.

---

The standard sizes

Memorise the M3 row. It is most of an FTC robot.

Thread	Tap drill	Close clearance	Free clearance
M3 x 0.5	2.5 mm	3.2 mm	3.4 mm
M4 x 0.7	3.3 mm	4.3 mm	4.5 mm
M5 x 0.8	4.2 mm	5.3 mm	5.5 mm
M6 x 1.0	5.0 mm	6.4 mm	6.6 mm

Two rules generate the whole table:

tap drill      = major diameter - pitch
clearance hole = major diameter + 0.2 mm  (close)
                 major diameter + 0.4 mm  (free)

Close fit where the part must locate accurately and you can afford to fight it slightly during assembly. Free fit where the part is one of several in a stack, or where a slot would have been better anyway.

1BringThe thread size the joint uses.

2ChangeThe thread, and compare how close the four diameters actually are.

3ReadThe gap between tap drill and clearance. It is smaller than it feels.

Tap Drill and Clearance Reference

Two different holes. Pick the wrong one and the joint is ruined.

ThreadM3 x 0.5M4 x 0.7M5 x 0.8M6 x 1.0#6-32 UNC#8-32 UNC#10-32 UNF1/4-20 UNC

M3 x 0.5 to scale

Tapped hole (smaller than the screw)Clearance hole (larger)

The tap drill and the clearance hole differ by only 0.70 mm, which is why they are so easily swapped. Mark every hole on the drawing as TAP or CL before anyone picks up a drill.

2.50 mmTap drill0.098 in, for a 75% thread

3.2 mmClose clearanceTight location, less adjustment

3.4 mmFree clearanceEasier assembly, some slop

2.50 mmMajor minus pitchThe rule of thumb, for comparison

Thread	Pitch	Tap drill	Close fit	Free fit
M3 x 0.5	0.50 mm	2.50 mm	3.2 mm	3.4 mm
M4 x 0.7	0.70 mm	3.30 mm	4.3 mm	4.5 mm
M5 x 0.8	0.80 mm	4.20 mm	5.3 mm	5.5 mm
M6 x 1.0	1.00 mm	5.00 mm	6.4 mm	6.6 mm
#6-32 UNC	0.79 mm	2.71 mm	3.8 mm	4.0 mm
#8-32 UNC	0.79 mm	3.45 mm	4.4 mm	4.6 mm
#10-32 UNF	0.79 mm	4.04 mm	5.1 mm	5.3 mm
1/4-20 UNC	1.27 mm	5.11 mm	6.7 mm	7.0 mm

The default FTC fastener. Used across REV and goBILDA hole patterns.

A tapped hole receives the threads and must be drilled small. A clearance hole lets the screw pass through freely and must be drilled large. Drilling a clearance hole where you needed a tapped hole cannot be undone, so mark which is which on the drawing before anyone picks up a drill.

Values are not saved. Nothing is sent anywhere.Open in the workbench

---

When 0.3 mm is not enough

The floor assumes one hole through one part. Add parts and the position errors stack, as in Lesson 4.4.

• Two plates drilled separately: use free clearance, or clamp and drill them together.
• Three or more holes in a pattern: make one hole close fit to locate, and slot the rest. Trying to hold position on four holes at once is how a part ends up unusable.
• A part you cannot re-make: slot it. A slot costs nothing at design time and saves the part.

The slot is the professional answer

Designing every hole round and then filing one out is the amateur version of the same decision. Deciding in CAD which hole locates and which one adjusts takes thirty seconds and produces a part that assembles.

---

Printed and laser cut holes

The 0.15 mm rule is about the fastener. The process adds its own error on top.

• FDM printed holes come out undersize, typically 0.1 to 0.3 mm on the diameter. Design them oversize deliberately, or drill after printing.
• Laser cut polycarbonate moves with the kerf and the heat affected edge. Cut a test coupon before committing a plate.
• Drilled aluminium comes out oversize, so a drilled hole is already closer to clearance than the drill size suggests.

Never assume the nominal. Measure one, then design against what your shop actually produces.

---

Fill-in-the-Blank Practice

1. The minimum clearance for a screw is __________ mm per side.
2. The M3 clearance hole is __________ mm and the M3 tap drill is 2.5 mm.
3. When three or more holes form a pattern, make one hole locate and __________ the rest.

Show answers

1. 0.15 (0.3 mm on the diameter)
2. 3.2 (close fit; 3.4 mm free)
3. slot

---

Exercise

Measure the last three holes your team drilled for M3 screws. Record each diameter. Anything under 3.2 mm is a joint that cannot clamp properly, and anything over about 3.6 mm is a joint that will not locate.

Ready to move on?

Only mark complete if you genuinely understand the material. Your progress will be saved in this browser.

Stuck on this lesson?

Ask about anything on this page. It can see which lesson you have open and which part you are reading.