Engineering Drawing Interpretation: Common Sources of Error

Why drawings are misread

A drawing is a compressed document. It relies on conventions set out in standards such as ASME Y14.5, ASME Y14.3 and the ISO 128 series, and on notes and title-block fields that change the meaning of every dimension on the sheet. A reader who misses one convention can read every number correctly and still build the wrong part.

None of the errors below is exotic. Each produces plausible geometry, which is why they survive to the shop floor.

First-angle and third-angle projection

Orthographic views can be arranged in two ways, both defined in ISO 5456-2. In first-angle projection each view is drawn on the opposite side of the front view from where it was seen: the top view goes below, the view from the left goes on the right. In third-angle projection each view is drawn on the side it was seen from. Third-angle is the ASME Y14.3 default and United States practice; first-angle is common in European and other ISO-based practice (Japanese practice uses third-angle).

A drawing read in the wrong system mirrors features between views. A counterbore on the left face lands on the right face, and on a nearly symmetric part nothing looks wrong until it does not fit its mate.

• Find the projection symbol, normally in or next to the title block. It shows a truncated cone in side view and in end view. In the third-angle symbol the end view sits on the side of the cone's small end; in the first-angle symbol it sits on the side of the large end.
• If there is no symbol, do not assume the system from the country the drawing came from. Check the arrangement against a feature that exists on one face only, such as a blind hole, a chamfer or a flat, and confirm it is consistent in every view.
• Views placed elsewhere on the sheet with a label (VIEW A, or a viewing arrow) are not governed by the arrangement rule. Read the label.

Units and number formats

A dimension without a unit is in the drawing's unit, stated in the title block or a general note. Assume the wrong one and the part is 25.4 times too large or too small, which is usually caught. The errors that survive are smaller.

• Decimal marker. Many ISO drawings use a comma as the decimal marker, so 12,5 is twelve and a half millimeters. Read with the comma as a thousands separator, 1,250 becomes 1250 instead of 1.25.
• Leading zeros. ASME Y14.5 writes millimeter values below one with a leading zero (0.5) and inch values without one (.50). A value written .5 on a millimeter drawing points to a drafting error worth a question.
• Dual dimensions. On a dual-dimensioned drawing, one unit is primary and the other is a conversion shown in brackets or below. Building from the converted value adds rounding the designer never specified.
• Implied precision. In inch practice the number of decimal places often selects the general tolerance (.XX against .XXX). Converting 1.250 in to 31.75 mm keeps the number and loses the tolerance it carried.

Convert with the exact factor (25.4 mm per inch) and carry the limits across, not only the nominal. The unit converter and the limit dimensions tool help with the arithmetic.

Scale, and dimensions not to scale

The scale in the title block (1:2, 2:1) says how the views were drawn. It does not make the sheet a measuring instrument. A PDF may have been printed to fit a different paper size, a detail view may carry its own scale, and a dimension may have been edited without the geometry being redrawn. That is why many title blocks carry the note DO NOT SCALE DRAWING.

• A dimension underlined with a thick straight line is not drawn to scale: the number governs and the picture does not. ASME Y14.5 and ISO 129-1 both use this marking. Some drawings write NTS instead.
• Detail views carry their own scale (DETAIL B, SCALE 4:1). On a 1:1 sheet, reading a 4:1 detail at the sheet scale makes a feature four times too large.
• A view shortened with break lines keeps its true overall dimension. The drawn length is not the part's length.

Hidden lines and section views

Hidden lines, drawn thin and dashed, show edges behind the visible surface. Drafters often leave them out where they would clutter a view, and both ASME and ISO practice allow that. A missing hidden line is therefore weak evidence. A hole drawn as a circle in one view, with no hidden lines in the next, may be blind, through, or simply not drawn there; the callout (THRU, a depth symbol, a depth value) decides.

Reading section views

• The arrows on a cutting-plane line point in the direction of viewing. Read backwards, the section puts features on the wrong side of the part.
• Hatching shows cut material. By convention, ribs, webs, shafts, bolts, pins and keys cut along their length are usually drawn without hatching, so an unhatched rib in a section is still solid.
• An aligned section rotates a feature, such as a hole on a bolt circle, into the cutting plane. It shows the hole's true distance from the axis, not its true angle. Read the angle from the end view.
• A removed section is drawn away from its cutting plane, sometimes at a different scale, so check its label and scale before reading it. A revolved section is drawn in place, rotated into the view, and can be mistaken for part of the outline.

Symbols that are misread

ASME Y14.5 defines the dimensioning symbols on ASME drawings, and ISO 7083 sets the proportions of geometrical tolerancing symbols. A symbol lost in a poor copy changes the value it belongs to.

Counterbores, countersinks and spotfaces

ASME Y14.5 uses symbols for the counterbore (⌴), the countersink (⌵) and depth (↧), so a counterbored hole reads like Ø6.6 THRU, ⌴ Ø11 ↧6.8. Many ISO drawings dimension it on a section or in a note instead. The depth is measured from the surface where the counterbore starts.

A countersink is called out by its diameter at the surface and its included angle: 90° for most metric countersunk screws, 82° for most inch flat-head screws. Cutting an 82° countersink for a 90° callout, or the reverse, seats the screw head on an edge instead of its cone. A spotface is shallower than a counterbore and exists to give a flat seat; ASME Y14.5 marks it with SF inside the counterbore symbol, and a spotface with no depth is cut only as deep as needed to clean up the surface.

Thread callouts

ISO 6410 sets how threads are drawn: the crest as a thick line and the root as a thin one, with the root shown in an end view as a thin circle of about three quarters. On an internal thread the thick circle is the minor diameter. A reader who takes it as the thread size gets roughly the tap drill, not the thread.

• M10 alone is the coarse thread, pitch 1.5. M10×1.25 is a fine pitch. Cutting the coarse thread for a fine-pitch callout makes a hole the mating screw will not enter.
• Tolerance classes are case-sensitive: 6H is an internal thread, 6g an external one.
• LH marks a left-hand thread. It sits at the end of the callout and is easy to miss.
• Unified threads read size, threads per inch, series and class: 1/4-20 UNC-2B is a quarter-inch internal thread, 20 threads per inch, class 2B (A is external, B internal).
• On a blind tapped hole, thread depth and drill depth are separate values. M6 ↧12 gives the thread depth; the drill depth is a separate callout or left to shop practice.

Superseded revisions

Every released change should raise the drawing's revision, shown in the title block and recorded in the revision block. ASME Y14.35 sets out the practice, and does not use the letters I, O, Q, S, X and Z as revision letters. A correct reading of the wrong revision is still a wrong part.

• Compare the revision in the title block with the revision on the purchase order or work order, not with the file name. A PDF named rev B can carry rev C in its title block, or the reverse.
• On a multi-sheet drawing, check the revision on every sheet. A sheet from an older print set is easy to mix in.
• A drawing marked PRELIMINARY or NOT FOR PRODUCTION, or with no approval, is not released. It is a reason to stop, not a source of dimensions.

General-tolerance blocks

Most dimensions carry no tolerance of their own. They take the general tolerance in the title block or a general note, the part of the sheet readers skip most often.

Three points catch readers out. A general tolerance does not apply to reference dimensions, basic dimensions, or dimensions with their own tolerance. The governing standard changes what a size tolerance controls: under ASME Y14.5, Rule #1 makes the limits of size also limit form (the envelope principle), while ISO 8015 applies the independency principle by default, so the same numbers can describe different parts. And ISO 2768-1 covers linear and angular dimensions only; general geometrical tolerances need a separate class, such as the K in ISO 2768-mK.

For fits and stacks, see the fit calculator, the tolerance stack-up tool and the guide to drawing tolerances and CAD.

Title-block data

The title block states the facts that apply to everything else. ISO 7200 defines its data fields; ASME Y14.100 sets out United States drawing practice, including what a drawing must state. Read these before the first view:

• Drawing number and part number. They are not always the same.
• Revision, and the sheet count. SHEET 1 OF 3 means two more sheets that may hold notes, sections or a flat pattern.
• Units, scale and the projection symbol.
• The general tolerance, and the standard the drawing is interpreted under, for example ASME Y14.5-2018 or an ISO reference such as ISO 8015.
• Material with its condition or temper, and the finish or coating. On a close fit, check whether the dimensions apply before or after coating.
• Release state, and proprietary or export-control notices, which say who may see the drawing.
• General notes, such as BREAK SHARP EDGES, and flag notes referenced from the views by a numbered symbol.

A checklist before you build

Questions engineers ask