How to Read a Technical Drawing: 8 Steps for CNC

Over eleven lessons we have taken technical drawing apart rule by rule. This last lesson puts it back together into one skill: how do you read a drawing you have never seen before, and how do you turn what it says into decisions at the machine?

Reading a drawing as a machinist is not the same as drawing one as a draughtsman. The machinist converts the drawing into manufacturing decisions: which face is the reference, which dimension is critical, which operation comes first.

Reading order: eight steps

The commonest mistake is to look at a drawing and start reading dimensions immediately. A dimension read before you understand what the part is gets misinterpreted. Keep this order:

Figure 12.1 — The eight steps of reading a technical drawing. Break the order and mistakes follow.

Read the title block. Material, scale, projection method (first or third angle), quantity, drawing number. Never take a size off the paper with a ruler — the scale is there for orientation, not measurement.
Match up the views. Which is the front, which the top, which the side? First and third angle place them in opposite positions; confuse them and you build a mirror image.
Build the shape mentally. Separate sections, hatching and dashed lines. Hatched area = solid material. Dashed line = hidden edge.
Find the overall dimensions. Greatest length, greatest diameter, total thickness. Raw material selection comes from these.
Mark the toleranced dimensions. H7, h6, ±0,05. These are the critical sizes; your measuring plan is built around them.
Read the surface symbols. The difference between Ra 0,8 and Ra 6,3 changes the process and the number of passes.
Read the geometrical tolerances. Perpendicularity, parallelism and position frames drive the workholding plan directly.
Check the notes and standard parts. Heat treatment, coating, chamfers, “general tolerances ISO 2768-m” — the most frequently overlooked part of any drawing.

A worked example

The drawing below brings together everything from the previous lessons on one sheet: a section view, diameter dimensioning, ISO fits, surface texture, a geometrical tolerance and a bolt circle.

Figure 12.2 — A flanged bush. Section view on the left, side view on the right.

What you see	What it means	What it means at the machine
C45 / Qty 1 / Scale 1:2	Medium carbon steel, one off, drawn half size	Raw bar Ø95 × 62 mm
Ø90	Flange outside diameter, no tolerance given	General tolerance — ±0,3 to ISO 2768-m
Ø60 h7	Shaft basis, upper deviation 0, lower −0,030	Precision turning; measure with a micrometer, not a caliper
Ø35 H7	Hole basis, lower deviation 0, upper +0,025	Drill → Ø33 → ream or fine bore
12 and 57	Flange thickness and overall length	Z axis steps
4× Ø9 on Ø75	Four fixing holes at 90° spacing	Index 90°; hole centre radius 37,5 mm
Ra 1,6 (bore)	Finely finished surface	Rough turning will not reach it — ream or fine pass needed
Ra 3,2 (general)	Applies to all other surfaces	Normal finishing pass is enough
⊥ 0,05 A	Flange face square to datum A, the bore axis	Machine flange face and bore in one setting
Chamfer 1×45°	Break the sharp edges	Chamfer tool or chamfer cycle

Do not memorise tolerance values — learn the logic. Capital H = hole, lower case h = shaft. The lower deviation of H7 is always 0 (a hole is never smaller than nominal). The upper deviation of h7 is always 0 (a shaft is never larger than nominal). The smaller the grade number, the tighter the zone. Details in Lesson 8.

Getting the datum and the operation sequence from the drawing

A drawing never states the workpiece zero point directly — but it does tell you which face is the reference. There are two places to look:

The face the dimensions start from. In parallel dimensioning every size is taken from one face; that face is the designer’s reference.
The datum letters (A, B, C). A datum used in a geometrical tolerance is the functional reference of the part. Setting up from it is the easiest way to hold the tolerance.

Figure 12.3 — Choosing the zero point on the same part, and the operation sequence read from the drawing.

In the example, datum A is the bore axis and the flange face must be perpendicular to it. Taken together those two facts say one thing: machine the flange face and the bore in a single setting. Remove the part and turn it round, and holding 0,05 mm of perpendicularity becomes a matter of luck.

Choosing the measuring instrument from the tolerance

Tolerance width	Suitable instrument
0,5 mm and above	Vernier caliper (0,05 / 0,02 mm)
0,1 – 0,5 mm	Digital caliper
0,02 – 0,1 mm	Micrometer (0,01 mm)
0,01 – 0,02 mm	Micrometer + dial gauge, internal micrometer
below 0,01 mm	Gauges, comparator fixture, CMM

The rule of thumb: the resolution of the instrument should be no more than one tenth of the tolerance width. A 0,025 mm H7 tolerance cannot be measured with a caliper reading to 0,05 mm.

Common drawing-reading mistakes

Measuring off the paper. Even at 1:1, printing and copying change the size. If a dimension is missing, ask for it.
Confusing first and third angle. Check the symbol in the title block. Get it wrong and you make a mirror image.
Missing the Ø symbol. “Ø40” is a diameter, “40” is a length. In a section they can look alike.
Confusing radius and diameter. R20 and Ø20 differ by a factor of two.
Assuming an untoleranced dimension has no tolerance. It is covered by the general tolerance standard named in the title block.
Ignoring surface symbols. The Ra value decides the process and the number of passes.
Mistaking a dashed line for a section. Dashed = hidden edge; a section is a hatched area.

Test yourself

Which is the most critical dimension in Figure 12.2?
Ø35 H7 — a 0,025 mm tolerance plus an Ra 1,6 surface requirement.
What are the limits of Ø60 h7?
Upper deviation 0, lower −0,030 → 59,970 – 60,000 mm.
What does “Ø75 bolt circle” mean?
The centres of the four holes lie on a circle of 75 mm diameter about the part axis — radius 37,5 mm, 90° apart.
How does ⊥ 0,05 A affect the setup?
The flange face and the bore must be machined in one setting, or the perpendicularity cannot be guaranteed.
What does “unspecified surfaces Ra 3,2” mean?
Ra 3,2 applies to every machined surface that carries no symbol of its own.
Can a 0,02 mm tolerance be measured with a 0,02 mm caliper?
No. The instrument resolution should be about a tenth of the tolerance — roughly 0,002 mm here.
The scale is 1:2 and a dimension is missing. What do you do?
You do not measure it and double it. You ask the drawing office.

Series complete. From Lesson 1 to here: paper and title block, line types, geometric constructions, projection, sections, dimensioning, surface texture, dimensional tolerances, geometrical tolerances, pictorial drawing and sketching, assembly and detail drawings, and finally drawing reading. You can now read a technical drawing from beginning to end. What follows is practice — read every drawing you meet with these eight steps.