14.3 Dimensioning, BOM, Projection Standards & GD&T

Certified SOLIDWORKS Associate CSWA

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1 Exam Overview & Logistics

1.1 Current Exam Facts & Format 1.2 Scoring, Points, Passing Score & Retakes 1.3 Time Management & Modeling Question Strategy

2 Workspace, Units & Design Intent

2.1 Interface & FeatureManager Tree 2.2 Document Units & MMGS Discipline 2.3 Design Intent Principles for CSWA

3 Sketch Foundations

3.1 Sketch Entities 3.2 Geometric Sketch Relations 3.3 Dimensions & Fully Defined Sketches

4 Sketch Construction Tools

4.1 Convert Entities, Offset & Mirror 4.2 Trim, Extend & Sketch Fillet/Chamfer 4.3 Construction Geometry & Sketch Planes

5 Extrude Boss & Cut

5.1 Extrude Boss/Base End Conditions 5.2 Extrude Cut Strategies 5.3 Contours, Thin Features & Common Extrude Traps

6 Revolves, Sweeps, Lofts & Edge Treatments

6.1 Revolve Boss & Revolve Cut 6.2 Sweep Boss/Base & Sweep Cut 6.3 Loft Boss/Base & Loft Cut 6.4 Fillet Features 6.5 Chamfer Features

7 Shell, Draft & Holes

7.1 Shell Feature 7.2 Draft Feature 7.3 Hole Wizard Fundamentals

8 Patterns & Mirror

8.1 Linear Pattern 8.2 Circular Pattern 8.3 Mirror Feature & Pattern Strategy 8.4 Fill Pattern & Choosing the Right Pattern Tool

9 Intermediate & Advanced Part Workflows

9.1 Multi-Feature Construction Order 9.2 Sketch Offset & Complex Profile Techniques 9.3 Editing, Rollback & Parent-Child

10 Materials & Mass Properties

10.1 Applying Materials & Density 10.2 Mass, Volume & Surface Area 10.3 Center of Mass, Coordinate Systems & Traps

11 Reference Geometry

11.1 Reference Planes 11.2 Axes, Points & Coordinate Systems 11.3 Mate References

12 Assembly Creation Basics

12.1 Inserting Components & Fixing the Base 12.2 Coincident, Concentric, Parallel, Perpendicular 12.3 Distance, Angle & Tangent Mates 12.4 Degrees of Freedom & Mate Diagnostics

13 Assembly Analysis & Advanced Mates

13.1 Advanced Mates Overview 13.2 Interference Detection 13.3 Assembly Mass Properties & Key Parameter Mods

14 Drafting Competencies

14.1 Standard & Projected Drawing Views 14.2 Section, Detail & Auxiliary Views 14.3 Dimensioning, BOM, Projection Standards & GD&T

14.3 Dimensioning, BOM, Projection Standards & GD&T

Key Takeaways Explain This Topic AI

Smart Dimension places drawing dimensions; Insert Model Items imports dimensions/annotations from the model—know both names for CSWA theory and that dimensions should not be blindly duplicated.

Balloons identify components; a Bill of Materials (BOM) table lists item numbers, quantities, and part data for assemblies—title block fields hold drawing identity (name, scale, projection, revision) conceptually.

Projection standard (1st vs 3rd angle) often appears as a symbol or template property—pair with 14.1: ANSI US default is third-angle.

Associate-level GD&T recognition: flatness, perpendicularity, position, datum feature symbols, and MMC modifier meaning—not full GDTP application depth.

Common traps: wrong projection type, misidentifying view type, ignoring hatch meaning, and confusing geometric tolerance symbols with ordinary size dimensions.

Last updated: August 2026

14.3 Dimensioning, BOM, Projection Standards & GD&T

Quick Answer: Use Smart Dimension (and Model Items ) to place size/location dimensions on views; use balloons + Bill of Materials for assembly callouts; read title block fields and projection symbols for standards; recognize basic GD&T symbols ( flatness, perpendicularity, position , datum feature , MMC ) at associate level—identification, not full tolerance stack analysis.

Views without dimensions and notes are incomplete manufacturing documents. CSWA does not require you to fully detail a production drawing under the clock the way a drafting job would, but the Drafting Competencies items expect you to know what tools and symbols mean . This section finishes that vocabulary.

Dimensioning tools in SOLIDWORKS drawings
Smart Dimension

On a drawing sheet, Smart Dimension (same family as sketch Smart Dimension) attaches dimensions to view geometry: edges, vertices, hole diameters, angles between lines, etc. You click entities in a view , place the dimension text, and the dimension stays associative to the model—change the part, and driving model dimensions update; drawing dimensions that reference model geometry update after rebuild.

Action Typical result
Dimension two parallel edges Linear distance
Dimension a circle Diameter (Ø)
Dimension a radius arc Radius (R)
Dimension two lines Angle
Dimension to a hole center Location dimension

Exam angle: Questions may ask which tool adds dimensions on a drawing. Smart Dimension is the primary answer. Marking menu / annotation toolbar placement still counts as Smart Dimension workflow.

Model Items

Insert → Model Items brings dimensions, hole callouts, annotations, and reference geometry marks from the 3D model into selected drawing views. This is efficient when the part was fully dimensioned in sketches/features: you import rather than re-dimension everything by hand.

Method Pros CSWA theory note
Smart Dimension on drawing Precise control of what appears Manual placement skill
Model Items Fast import of existing model dims “Insert dimensions from the model”
Duplicating both blindly Clutter, dual dimensions Avoid double-dimensioning the same feature

Trap: Model Items can flood a view with every sketch dimension. Production practice cleans and rearranges; theory questions still test that Model Items imports model-based annotations/dimensions into the drawing.

Annotation types (conceptual list)

Beyond pure dimensions, drawings use:

Notes — text instructions, finish notes, general tolerances
Hole callouts — hole wizard-style threaded/simple hole specs
Center marks / centerlines — for holes and symmetry
Datum feature symbols — GD&T reference frames (below)
Geometric tolerance frames — feature control frames
Surface finish / weld symbols — may appear in figures; rare deep testing on CSWA
Balloons — item numbers for assemblies

You do not need every annotation PropertyManager option memorized—recognize what family an annotation belongs to when a figure is shown.

Balloons and Bill of Materials (BOM)
Balloons

Balloons (auto-balloon or manual) place circled item numbers on assembly drawing views. Each balloon points to a component instance and matches a row in the Bill of Materials .

Tool idea Function
Balloon One callout tied to a component
Auto Balloon Places balloons for components in a view in batch
Magnetic lines Align balloon leaders neatly (productivity; light theory)

If a question shows circled numbers on an assembly isometric with leaders to parts, those are balloons , not section labels (section labels pair with cutting lines) or detail labels (detail circles).

Bill of Materials table

Insert → Tables → Bill of Materials creates a BOM table on an assembly drawing. Typical columns:

Column (examples) Content
Item No. Matches balloon numbers
Qty Quantity of that component
Part Number / Description From file properties or custom properties
Material If mapped from properties

BOM is a table , not a view. It lists parts in the assembly (top-level or parts-only/ indented options in the PropertyManager). CSWA-level recognition: BOM = parts list table linked to balloons .

Title block fields (conceptual)

The title block (sheet format) holds drawing metadata. Concept-level fields:

Field Typical content
Drawing / part name Title of the document
Drawing number Tracking ID
Revision Change letter/number
Scale Sheet or primary scale
Drawn by / date Authorship
Material (part drawings) Stock material note
Projection symbol First- or third-angle
Units note mm / inch general note
Company approval blocks Sign-offs

SOLIDWORKS links many title block attributes to custom properties of the model or sheet. For CSWA, know that projection method and scale often live in the title block/format , and that third-angle vs first-angle may be indicated by symbol there (ties to 14.1).

Projection standards — drawing communication recap

Standard Template habit Top vs Front Side view habit
Third-angle ANSI / US default Top above Front Right view on the right
First-angle ISO Top below Front Right view on the left

CSWA MC pattern: “This title block shows which projection?” or “Which is default for US ANSI templates?” → Third-angle . Do not answer first-angle unless the figure is clearly ISO/first-angle layout or the stem says ISO.

GD&T at associate recognition level

Geometric Dimensioning and Tolerancing (GD&T) uses standardized symbols to control form, orientation, location, and runout beyond simple ± size tolerances. CSWA is not a GDTP certification—you need symbol recognition and basic meaning , not advanced bonus tolerance math for every case.

Feature control frame (concept)

A rectangular feature control frame holds:

Geometric characteristic symbol (e.g., flatness, position)
Tolerance value (and material condition modifiers if any)
Datum references (primary, secondary, tertiary as required)

Example structure (conceptual): [ ⟂ | 0.1 | A ] means perpendicularity within 0.1 relative to datum A (actual drawing frames use the proper symbol cells).

High-yield symbols for CSWA-style recognition

Symbol / name Category Plain-language meaning

Flatness (parallelogram symbol) Form Surface must lie between two parallel planes a stated distance apart; no datum required for basic flatness

Perpendicularity (⊥) Orientation Feature must be 90° to a datum within tolerance
Position (⊕) Location Axis or center plane location relative to datums (true position)
Datum feature symbol Reference Identifies a feature as datum A, B, C , … for other controls

MMC (Ⓜ) Modifier Maximum Material Condition — tolerance applies at the state of maximum material (e.g., smallest hole, largest pin); can allow bonus tolerance as feature departs from MMC

Datums

A datum is a theoretically exact reference (plane, axis, point) established from a datum feature on the part. The datum feature symbol on the drawing points to the real feature (a face, a hole, etc.). Position and perpendicularity frames commonly reference datums; flatness as pure form often does not.

MMC intro (associate depth only)

Maximum Material Condition (MMC) is the condition where the feature contains the maximum amount of material within size limits:

For a pin/external feature: MMC ≈ largest size
For a hole/internal feature: MMC ≈ smallest size

The Ⓜ modifier in a feature control frame means the geometric tolerance is stated at MMC; as the actual feature size leaves MMC (hole gets larger, pin gets smaller), bonus tolerance may become available. CSWA may only ask you to identify MMC or know it relates to material condition—not to compute a full stack.

LMC (Least Material Condition, Ⓛ) is the opposite idea; know the name exists. RFS (Regardless of Feature Size) is implied when no material condition modifier is shown on many controls—recognize that absence of Ⓜ/Ⓛ often means RFS at associate level if asked.

Size dimension vs geometric control

Callout type Controls
Ordinary dimension 20 ± 0.1 Size (and basic location if a chain of sizes)
Flatness 0.05 on a face Form of that surface
Perpendicularity to A Orientation vs datum
Position of hole pattern to A|B|C Location of features

Trap: Treating a position frame as “just another diameter dimension.” Diameter still needs a size dimension; position controls where the feature is relative to datums.

Putting annotations together on an assembly drawing

Typical associate-level assembly sheet content:

Isometric or multiview of the assembly
Balloons on components
BOM table with matching item numbers
Maybe a few overall dimensions or a note “SEE PART DRAWINGS FOR DETAILS”
Title block with scale, projection symbol, revision

Part drawings emphasize orthographics + sections/details + dimensions + GD&T more heavily than balloons/BOM.

Common CSWA drafting traps (full category)

Trap Wrong answer pattern Correct thinking
Wrong projection type Always pick first-angle ANSI US → third-angle
Misidentify view type Call detail a section Cutting line+hatch vs circle+scale
Hatch meaning Hatch = void Hatch = solid in cut
BOM vs balloon BOM is a view BOM is a table ; balloons are callouts
Model Items vs Smart Dimension Same button Model Items imports ; Smart Dimension places
GD&T flatness needs datum Always attach A|B|C Basic flatness is form-only
MMC = “tightest tolerance always” Ignore size interaction MMC is a material condition modifier on the frame
Exam-day drafting sprint (all of Chapter 14)

Step Look for Link
1 Relative Top/Right placement or projection symbol 1st vs 3rd angle (14.1)
2 View creation language (projected, standard 3, iso) Model / Projected (14.1)
3 Cutting line, hatch, half/full Section (14.2)
4 Circle + DETAIL + large scale Detail (14.2)
5 True size on incline Auxiliary (14.2)
6 Dimensions source Smart Dimension / Model Items (14.3)
7 Circled item numbers + parts table Balloons + BOM (14.3)
8 ⊥ ⊕ flatness Ⓜ datum flags GD&T recognition (14.3)
Study drills that transfer

Open any ANSI template drawing of a simple block: confirm third-angle symbol and Top-above-Front layout.

Add Standard 3 View , project an isometric, add a section , a detail at 2:1, and an auxiliary on a chamfered face—label each aloud.

Insert Model Items , then delete clutter and place two Smart Dimensions manually.

On an assembly drawing, Auto Balloon + BOM ; match item numbers.

Flashcard the five GD&T recognition items: flatness, perpendicularity, position, datum feature, MMC.

Drafting is only 15 points , but it is pure knowledge —no rebuild failures, no unit typos. Combined with strong parts and assemblies, these recognition skills protect the cut score. You have now closed the official CSWA skill map’s drafting category: views, specialized projections, and the annotation/BOM/GD&T language the associate exam expects you to read.