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Engineering Drawing Symbols and Standards: A Practical Guide for SolidWorks Users

Published Nov 03, 2026, updated Nov 03, 2026

13 min

Table of Contents
  • Which Standard Applies: ASME or ISO
  • Line Types and What They Mean
  • Dimension and Feature Symbols
  • Surface, Weld, Datum and GD&T Symbols
  • Scale and Projection
  • Reading a Callout Set: The Plate Example
  • Setting the Drafting Standard in SolidWorks
  • Where JLCCAN Fits
  • Common Symbol and Standard Mistakes
  • FAQ

Quick answer: Engineering drawing symbols are the shorthand that tells a reader the diameter, depth, thread, finish or tolerance of a feature without a paragraph of text. Which symbols to use depends on the drafting standard: ASME Y14 in the U.S., ISO in most other places. In SolidWorks the standard is set once under Document Properties > Drafting Standard, and the symbols are added with Smart Dimension, Hole Callout, the Surface Finish and Geometric Tolerance tools, or the Add Symbol button in notes.

Two engineers can draw the same bracket and produce drawings that look unrelated. One uses third-angle views and decimal inches, the other first-angle views and millimetres. Both are correct, and a reader who does not know which standard applies will misread one of them.

This guide is a reference for the symbols on mechanical drawings, grouped by what they do, with the standard behind each one and the SolidWorks tool that adds it. It also covers scale and projection, and finishes by reading a real callout set from the plate used in our other guides. For the surrounding workflow, see our guide to creating a SolidWorks 3D to 2D drawing.

Key Takeaways

  • Which symbols apply depends on the drafting standard, ASME Y14 or ISO, and it is set once under Document Properties > Drafting Standard and carried in the template.
  • ASME drawings normally use third-angle projection and ISO drawings first-angle, so a view on the unexpected side can be a standards difference and not an error.
  • Symbols without a keyboard key should be inserted with the Add Symbol option, because a look-alike character may not survive export.
  • Scale never changes dimension values, so a reader should take sizes from the dimensions and not from measuring the drawing.

Which Standard Applies: ASME or ISO

First-angle vs. third-angle projection symbols

A drafting standard is a rulebook for how a drawing looks and what its marks mean. Two families cover most mechanical work.

  • ASME Y14 is the American series. ASME Y14.5 covers dimensioning and tolerancing, and the rest of the Y14 family covers views, drawing types, parts lists, revisions and surface texture symbols.
  • ISO is the international series, used across Europe and most of Asia. ISO 128 sets the general principles for technical drawings, with separate standards for dimensioning, tolerancing, sheets, scales and title blocks.
  • National standards (DIN, JIS, BSI, GB, GOST) exist too, and most of them are close to ISO. Here are the standards you will meet most often, with the area each covers.
AreaASMEISO
General drawing practice, lines and viewsASME Y14.3, Y14.24, Y14.100ISO 128 series, ISO 5456 (projection methods)
Dimensioning and tolerancingASME Y14.5ISO 129-1 (dimensioning), ISO 1101 (geometrical tolerancing), ISO 2768 (general tolerances)
Sheet sizes and layoutASME Y14.1ISO 5457
Title block dataASME Y14.100ISO 7200
ScalesPer Y14 practiceISO 5455
Surface texture symbolsASME Y14.36 (with ASME B46.1)ISO 1302, now ISO 21920-1
Threads in drawingsASME Y14.6ISO 6410
Parts listsASME Y14.34Per ISO 7573
The table is a map and not a substitute for the standards. Editions change, so check the current one before you quote a clause. For title block fields and sheet sizes, see our title block guide.
The differences that catch people out most often:
  • Projection. ASME drawings normally use third-angle projection and ISO drawings normally use first-angle, so a view placed on the "wrong" side is a standards difference, not an error. The drawing carries a projection symbol so the reader knows.
  • Units and notation. Inch drawings and millimetre drawings use different conventions for decimals and tolerances.
  • Callouts. Thread and hole notes are written differently (M6×1 against 1/4-20 UNC, for example), and SolidWorks changes some callout behaviour with the standard, as noted in our Hole Wizard guide.

Line Types and What They Mean

Before any symbol, the lines carry meaning. A drawing is read first by its line weight and pattern.

LineAppearanceMeaning
Visible (object) lineThick, continuousOutline of what you can see
Hidden lineMedium or thin, dashedEdges behind a surface
Center lineThin, long and short dashesAxis of a hole, shaft or symmetric part
Dimension and extension linesThin, continuousCarry the dimension, never part of the object
Cutting plane lineThick, with arrowheads at the endsWhere a section view is taken
Section (hatch) linesThin, continuous, usually at 45°Cut material in a section view
Break lineThin, freehand or zigzagPart is shortened to save space
Phantom lineThin, long dash and two short dashesAlternate positions or adjacent parts
In SolidWorks, the Line Format toolbar changes the style and thickness of a selected line, and Document Properties > Line Font sets the defaults for each line type. If your hidden lines look the same as visible lines, the fault is almost always in those defaults and not in the views.

Dimension and Feature Symbols

These are the marks you use on almost every part. Where a glyph does not exist on a keyboard, drawings use an abbreviation.

Mechanical dimensions and feature symbols on a drawing

Symbol or abbreviationMeaningExampleIn SolidWorks
ØDiameterØ6.6Added automatically by Smart Dimension on circles
RRadiusR5Smart Dimension on arcs
SR / SØSpherical radius or diameterSR12Dimension text symbols
±Plus or minus tolerance20 ±0.1Tolerance settings in the dimension
°Degrees45°Angular dimension
× (after a number)Number of instances6× Ø6.6Hole callout counts instances
THRUHole goes all the way throughØ6.6 THRUHole Wizard end condition
TYPTypical, repeats elsewhereR3 TYPText in the dimension
( )Reference dimension(80)Driven dimension in parentheses
Boxed numberBasic dimension, toleranced by geometry[20]Basic dimension option
CBORE, CSKCounterbore, countersinkCBORE Ø11 × 6.5Hole Wizard hole callout
M6×1Metric thread, size × pitchM6×1 ↓ 12Cosmetic thread callout
Depth symbolDepth of a hole or pocket↓ 12Hole callout and dimension text
□Square feature□10Dimension text symbols
Chamfer noteDistance × angle1 × 45°Chamfer Dimension
The rules behind how to place these (once per feature, outside the view, from a datum) are covered in our SolidWorks dimensioning. Reference dimensions and chamfer dimensions each have their own guide: reference dimension guide and chamfer dimension guide.
To add a symbol that has no keyboard key, double-click the note or dimension text and use the Add Symbol option in the Note PropertyManager (or the symbol list in the dimension text box). Symbols inserted this way stay as symbols when the drawing is exported, which typing a look-alike character does not guarantee.

Surface, Weld, Datum and GD&T Symbols

These four families are specialist topics. Each gets one line here.

FamilyWhat it statesIn SolidWorksDeeper reference
Surface textureRoughness (Ra) and finish requirementsSurface Finish tool, Annotation tabSurface roughness symbols, JLCCNC
WeldType, size and location of a weldWeld Symbol tool, Annotation tab (or Insert > Annotations > Weld Symbol)Our weldment drawing guide
Datum feature and targetThe reference a part is located and measured fromDatum Feature toolGD&T in CNC machining, JLCCNC
Geometric toleranceForm, orientation, location and runout limitsGeometric Tolerance toolGD&T flatness, true position
One SolidWorks point worth knowing. The drafting standard changes how these symbols are drawn, so a surface finish symbol under ISO and one under ANSI are not interchangeable even when the value is the same.

Scale and Projection

Scale is the ratio between the size of the drawn view and the real part. It does not change the dimension values, which always state the real size, and a reader should never measure a drawing to find a dimension.

ISO 5455 recommends a short list of ratios.

TypeCommon ratios
Full size1:1
Reduction1:2, 1:5, 1:10, 1:20, 1:50, 1:100
Enlargement2:1, 5:1, 10:1, 20:1, 50:1
Other ratios are used, but sticking to the list keeps drawings consistent across a team. A view that is not drawn to scale is marked as such, typically with the note NTS (not to scale).
In SolidWorks there are two places to set scale, and mixing them up causes most of the "my view is the wrong size" questions.
  • Sheet scale is set in the sheet properties (right-click the sheet, choose Properties). New views take this scale by default.
  • View scale is set in the view's own PropertyManager. Choose between using the sheet scale, the parent scale (for detail and projected views) or a custom scale.
  • A detail view is the one place a custom scale is the norm. It magnifies a small region, and its label shows its own scale.
  • The type of projection (first angle or third angle) is also a sheet property, and it is saved in the drawing template and not in the sheet format, as covered in our drawing template guide.

Reading a Callout Set: The Plate Example

Here are the marks you would find on the 120 × 80 × 10 mm plate used in our dimensioning and hole guides, with what each one tells the shop.

On the drawingMeaningStandard areaSolidWorks tool
120, 80, 10Overall size in millimetresDimensioningSmart Dimension or Model Items
4× Ø6.6 THRUFour clearance holes, throughHole calloutHole Wizard, Hole Callout
2× M6×1 ↓ 12Two tapped holes, thread depth 12Thread calloutCosmetic thread
(80)Reference dimension, not tolerancedDimensioningDriven dimension
1 × 45°Edge breakChamferChamfer Dimension
Surface symbol with Ra 3.2Machined surface, roughness limitSurface textureSurface Finish
Datum feature AThe left edge the plate locates onDatumDatum Feature
A–A with thick arrowed lineSection taken at that planeViews and linesSection View
Projection symbolFirst or third angleSheet propertySheet properties
Every row maps to a standard and a tool. When something on a drawing looks unfamiliar, finding which row it belongs to usually answers it.

Setting the Drafting Standard in SolidWorks

Open Options, choose the Document Properties tab and select Drafting Standard. The overall drafting standard can be ANSI, ISO, DIN, JIS, BSI, GOST or GB, or a custom standard you create. Each time you pick one, the base standard of every detail (dimensions, notes, balloons, tables and so on) updates to match.

SolidWorks drafting standard settings

Three practical points from SolidWorks Help.

  • A custom standard is a saved set of annotation settings. You can copy, rename, export it to a file and load it on another machine, which is the simplest way to give a team one company standard.
  • Not every setting travels with the standard. SolidWorks Help says the standard copies annotation settings, and the remaining document properties are saved with the drawing template. A custom standard on its own will not make two machines agree. The template has to carry the rest.
  • Changing the standard on an existing drawing changes how its annotations draw. Review dimensions, balloons and callouts afterwards, because arrowheads, text placement and symbols can shift.
  • The working rule: choose the standard first, put it in the template, and keep one template per standard. A drawing that starts under ANSI and is switched to ISO halfway often ends up with mixed conventions.

Where JLCCAN Fits

Standard drawings repeat the same symbols on every part, which is where a plugin helps. JLCCAN's features page lists Auto Drawing & Dimensioning, which generates drawings from 3D models and applies linear dimensions, dimension chains, hole tables, GD&T and surface finish annotations in batch, and a Rotate View tool in the drawing tools. Batch Manager is listed for title block replacement, which matters when a standard or company format changes.

The product team confirmed how the automatic annotations behave. They follow the GB standard, the Chinese national standard, so for ANSI or ISO drawings the generated annotations need a review against the standard the customer asked for. They are inserted as native SolidWorks annotations, and the symbols covered are surface roughness, parallelism, perpendicularity, flatness, coaxiality, symmetry, circular runout and total runout. JLCCAN does not have a weld symbol function, so weld symbols are added with SolidWorks' own Weld Symbol tool.

The reviewing step does not change with automation. Whoever releases the drawing should still check that the symbols match the standard the customer asked for.

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Common Symbol and Standard Mistakes

  • Mixing first-angle and third-angle views on one drawing. The projection symbol says one thing and the layout says another.
  • Typing look-alike characters. A letter O for a diameter sign or a lowercase x for the multiplication sign may not survive export. Use the symbol tool.
  • Using an ISO surface finish symbol on an ASME drawing, or the reverse. The shapes and rules differ.
  • Setting the standard after the drawing is finished. Switch it first, or review every annotation afterwards.
  • Measuring the drawing. Scale is for reading shapes. Dimension values state the size.
  • Overriding line weights by hand. Hand-edited weights drift. Fix the defaults in Document Properties > Line Font.
  • Copying symbols from a chart for the wrong discipline. Electrical, piping and architectural charts use different symbols. Use a mechanical chart.

FAQ

What are the most common symbols on a mechanical drawing? Diameter (Ø), radius (R), plus or minus (±), the number of instances (for example 4×), THRU, thread callouts such as M6×1, chamfer notes, surface finish symbols and datum symbols.

What is the difference between ASME and ISO drawing standards? ASME Y14 is the American series, with Y14.5 covering dimensioning and tolerancing, and it normally uses third-angle projection. ISO is the international series, with ISO 128 and related standards, and it normally uses first-angle projection. Callouts, symbols and notation also differ in detail.

How do I choose the drafting standard in SolidWorks? With a drawing open, go to Options > Document Properties > Drafting Standard and pick ANSI, ISO, DIN, JIS, BSI, GOST, GB or a custom standard.

How do I change the scale of a view in SolidWorks? Change the sheet scale in the sheet properties to rescale views that follow it, or select a view and set a custom scale in its PropertyManager.

How do I insert a diameter or other symbol in a SolidWorks drawing? Dimensions on circles get the diameter symbol automatically. For notes and text, double-click to edit and use the Add Symbol option, so the symbol stays a real symbol.

Which standard should my drawings follow? The one your customer or company specifies. If none is specified, pick one, set it in the template and apply it to every drawing.

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