Guide · Manufacturing

Drawing tapped holes, clearance holes, counterbores and countersinks correctly

7 min read · updated 3 Nov 2026

Holes are the most common feature on part drawings — and the most often drawn wrong. From the drawing alone the machinist must know whether a hole is tapped or plain, its size, its depth and how many there are. The rule: draw the hole by the standard, then write a complete note on one line, such as 4× M6 depth 12 / drill Ø5 depth 15.

How to draw threads (ISO 6410)

Drawings do not show individual thread turns; they use a simple convention:

Internal thread, seen end-on: a thick circle at the tap drill size (thread root) and a thin circle of about three quarters at the thread size. M6 = thick Ø5 circle + thin ¾ Ø6 arc.
External thread (screw, shaft) seen from the end: a thick circle at the thread size and a thin ¾ circle at the root diameter.
Tapped hole in section: thick lines at the drill size, thin lines at the thread size, hatching up to the thick lines, and a 120° cone at the bottom of the drilled hole.
The end of the thread length is a thick line across the hole.

Tap drill and clearance hole table (metric coarse threads)

Thread	Pitch (mm)	Tap drill Ø	Clearance, fine Ø	Clearance, medium Ø
M3	0.5	2.5	3.2	3.4
M4	0.7	3.3	4.3	4.5
M5	0.8	4.2	5.3	5.5
M6	1.0	5.0	6.4	6.6
M8	1.25	6.8	8.4	9.0
M10	1.5	8.5	10.5	11.0
M12	1.75	10.2	13.0	13.5

Tap drill ≈ thread size − pitch. Clearance holes follow ISO 273: fine where position must be accurate, medium for general use with more room for position error. Laser-cutting shops often add a little more on thin sheet; ask them first.

Advertisement · In-article

Writing complete hole notes

Hole	Example note	Meaning
Through tapped	`4× M6 THRU`	Four M6 threads through the full thickness
Blind tapped	`2× M8 depth 16 / drill Ø6.8 depth 20`	Thread 16 deep, drilled 20 deep (room for the tap's lead)
Fine thread	`M10×1`	Always state the pitch when it is not coarse
Clearance	`6× Ø6.6 THRU`	Medium clearance holes for M6
Counterbore	`4× Ø6.6 THRU / c'bore Ø11 depth 6.5`	Sinks an M6 socket head cap screw (ISO 4762) flush
Countersink	`4× Ø6.6 THRU / csk 90° Ø13`	For M6 flat head screws (ISO 10642), flush with the surface

The counterbore and countersink sizes are common values; always check them against the actual screw head from its datasheet.

Drawing and annotating holes in DXCAD2D Online

Draw an M6 tapped hole in the front view: press C, click the centre, type 2.5 (radius of Ø5) and Enter, on the thick-line layer.
Draw the thread arc: a ¾ arc of radius 3 on the thin-line layer. The easy way is a radius-3 circle trimmed (X) by the centre lines to remove one quarter, or a 3-point arc (A).
Add crossing centre lines on a layer set to the centre line type.
Group the finished hole (G), then copy it (CO) to other positions, or use Polar Array (PO) for holes on a circle.
Write the note with a leader (LE): click the hole edge, click where the text goes, then type, e.g. 4× M6 THRU.
Dimension the hole positions from the datum edges with D. Do not dimension the diameter again — it is in the note.

Laser cutting: a laser shop cannot cut threads. In the DXF for cutting, draw a plain circle at the tap drill size (Ø5 for M6) and tap it afterwards, or note on the PDF that tapping is required. Holes smaller than the sheet thickness rarely cut cleanly — drill them instead. See preparing drawings for laser cutting.

Try it right now — a free 2D CAD in your browser. Nothing to install, no sign-up.

Open DXCAD2D Online