SolidWorks Drawings, GD&T, BOM, and eDrawings

SolidWorks · Drawing

Overview

No matter how perfect the 3D model is, the shop floor still machines from a single drawing. A SolidWorks drawing (.slddrw) is a parametric drawing bidirectionally linked to its parts/assemblies, so views and dimensions update automatically when the model changes.

That said, without solid fundamentals in templates, view composition, dimension management, GD&T, BOMs, and balloons, a drawing unravels in no time.

This guide works from a practical standpoint: drawing-template setup, the variety of view types, Hole Callouts, GD&T, BOMs, balloons and blocks, and sharing externally via eDrawings/xDesign. For shortcuts see 01-shortcuts-ui.md; for the part-modeling foundation see 02-part-modeling.md.

1. Drawing Templates — `.drwdot` and `.slddrt`

A SolidWorks drawing document is split across two files. Mixing up the concepts is how template management goes wrong.

File	Role
`.drwdot`	Drawing template. Holds document-wide settings (units, standards, layers, annotation defaults).
`.slddrt`	Sheet Format. The 2D geometry for the border, title block, and revision block.

Menu path: Tools → Options → Document Properties → Drafting Standard lets you pick ISO, ANSI, KS, or JIS. Dimensions, Notes, Arrows, and Line Font are then all set in one go to match that standard.

Title-block automation: If you embed link expressions like $PRPSHEET:{Description} in the Sheet Format's text fields, the title block auto-fills by reading the Custom Properties of the part each view references.

The company logo, project number, material, weight, drawing number, author, and revision can all be wired up at once.

Tip Always distribute the company-standard Sheet Format through a shared network path. If each engineer keeps their own copy in a personal folder, revision-block formats drift subtly over time, and PDF distributions repeatedly end up with "title blocks that differ from drawing to drawing."

2. Types of Drawing Views

You can create many views at once, but in practice a front view plus 2–3 auxiliary views as needed is the most common setup.

View	Purpose
Standard 3 View	Auto-generates front, top, and side views. Default for drafts.
Model View	Manually place a view from a chosen orientation.
Projected View	Orthogonal projection (up/down/left/right) from an existing view.
Auxiliary View	Perpendicular projection of an inclined face. For dimensioning inclined surfaces.
Section View	Cross-section view. Full / Half / Aligned / Offset / Broken-out, etc.
Detail View	Local magnification bounded by a circle or rectangle. Separates dimensioning in cramped regions.
Broken View	Omits the middle of a long part (shaft, profile) to save scale.
Crop View	Keeps only the needed region and crops away the rest.
Alternate Position View	Overlays another posture of a mechanism as a ghost on the same view.
Exploded View	Assembly disassembly diagram. Used with BOMs and balloons on assembly drawings.

Example menu path: Insert → Drawing View → Section.

Tip Learning the Aligned Section View pays off — it lets you unfold the section of rotationally symmetric parts (flanges, gear housings) without distortion. Even a flange with bolt holes arranged irregularly around the circumference projects into a single clean section.

Note A Detail View's scale can be set independently of the sheet scale. If the sheet is 1:2 but a Detail is set to 2:1, dimension-text sizes diverge, so you must annotate explicitly to prevent a mismatch between the "SCALE" value in the title block and the visual size.

3. Hole Callout

Holes created with the Hole Wizard generate accurate callouts automatically. A through hole shows as ⌀5 THRU, a tapped hole as M8x1.25, a counterbore as ⌀8.5 THRU ⌵ ⌀14 ⌴ 5.

Menu path: Annotation → Hole Callout → pick the circle (hole) on the drawing.

2020+ versions allow Hole Callouts to be attached directly to holes inside Section Views.
Legacy Holes (made by hand with an Extrude Cut) can produce inaccurate callouts. Where possible, rework them with the Hole Wizard.
Advanced Holes (stepped diameters) expand a single-line callout into multiple lines, listing dimensions per depth.

Tip If you want to add company-specific symbols around the callout text (φ instead of ⌀, ▽ for depth, etc.), type them directly in the text box. The underlying parametric dimension is preserved, so the values still update automatically when the model changes.

4. Dimensions — Primary and Secondary

Drawing dimensions come from two sources. Blending the concepts leads to dimensions that disappear or are mis-applied when the model is edited.

Type	Creation	Effect when deleted
Primary (owned by the model)	`Insert → Model Items` imports feature dimensions automatically	Deleting the feature dimension on the model side removes it from the drawing too
Secondary (drawing-only)	Manually written with `Smart Dimension`	Exists only on the drawing, no effect on the model

Other dimensioning styles:

Ordinate Dimension: Accumulated distances from a single baseline. Maps directly to the CNC baseline.
Chain Dimension: Automates continuous dimensions.
Baseline Dimension: Branches every dimension line from a single baseline.

Note Think carefully before deleting a dimension imported via Model Items. If the feature dimension itself disappears, you'll find yourself repeatedly re-entering it manually, wondering "why is there no dimension on the drawing?" As an alternative, Hide keeps the model dimension while visually hiding it on the drawing.

5. GD&T — Geometric Tolerances

Menu path: Annotation → Geometric Tolerance.

Datum Feature Symbol: Assign datums A, B, C, etc., to edges or axes.
Feature Control Frame: Symbol (position ⌖, flatness ▱, parallelism ∥, etc.) + tolerance value + datum combination.
MBD (Model Based Definition): If licensed, PMI (Product Manufacturing Information) can be applied directly to the 3D model itself, delivering manufacturing information without a drawing (adoption is progressing in aerospace, automotive, and MIL environments).

Practical note: Learning the notation for GD&T is only half the job — you must also consider the inspection method (CMM, gauge R&R). A value like 0.05 position tolerance makes a large difference in measurability and measurement cost. Reviewing with the quality team before releasing drawings is recommended.

6. BOM (Bill of Materials)

Menu path: Table → Bill of Materials.

BOM types:

Top-Level Only: Only top-level components — for managing commercial supply units.
Parts Only: Every part (no assembly entries) — for rolling up manufacturing stock.
Indented: Indented by level — the "design BOM" that follows assembly order.

Columns can be added freely. By default you get Item No., Part Number, Description, Quantity, and in practice teams add Custom Properties like Material, Weight, Surface Finish, Supplier, and Lead Time alongside them.

Tip Set the Part Number column based on a Custom Property rather than "Document Name" — this is the standard. Even when filenames change frequently, the BOM part numbers stay fixed.

Tip Setting the Part Number displayed when used in a bill of materials option (in part Configuration Properties) causes different Configurations of the same part to appear with different numbers on the BOM. Handy when a standard part is divided by length or diameter.

7. Balloons and Magnetic Lines

A balloon points to a component in a view and links a BOM item number via a circular or rectangular symbol.

Auto Balloon: Auto-places across an entire view in circular, square, or grid patterns at once.
Stacked Balloon: Stacks multiple numbers vertically or horizontally. For when several parts (bolt + washer + nut, say) cluster at one point.
Magnetic Lines: Virtual lines that align balloons as if by magnet. When Auto Balloon placement comes out crooked, dragging balloons onto a line aligns them all at once.

Tip If the assembly has a Weldment Cut List, you can point the balloon's reference number at the Cut List Item number. On structural drawings, a balloon-plus-Cut-List-table combo is nearly standard for welded members.

8. Blocks — Reusable 2D Symbols

Frequently used 2D symbols (weld symbols, surface finish, bend symbols, custom center marks, company logos, etc.) are saved as Blocks and reused.

Location: Design Library → Annotations folder.
Create a custom Block: sketch → Tools → Block → Make → save as .sldblk.

Blocks can carry internal attributes, so you can drop the same Block in multiple places while varying only a reference number or value.

9. Tolerances, Annotations, and Sheet Layout

9.1 Tolerance Notation

General Tolerance: Noted in one place in the sheet's Note Block, e.g., "Unspecified tolerances per KS B ISO 2768-1 medium class." Removes the need to stamp a tolerance on every dimension and improves drawing readability.
Dimension Tolerance: Select a dimension → in the PropertyManager Tolerance/Precision section, choose Bilateral, Symmetric, Limit, Basic, or Min/Max.
Fit Tolerance: Specify ISO fit systems (H7/h6, etc.) directly in the Smart Dimension PropertyManager. Toggle between hole and shaft modes.

Tip Save your frequently used tolerance styles as Favorites so you don't re-enter the same tolerances every time.

9.2 Notes and Symbols

Note: Plain text. Model property values can be auto-inserted via $PRPSHEET:{property} format.
Surface Finish Symbol: Notates Ra/Rz values. Auto-aligns with leader lines and arrows.
Weld Symbol: Weld notation. Pick the standard between AWS and ISO.
Datum Target: Specifies point, line, or area datums.
Center Mark / Centerline: Auto-inserts on holes/circles (an option to apply to the entire view at once).

9.3 Working with Layers

Menu: Tools → Options → Document Properties → Line Font or the drawing Layer toolbar.

Place dimensions, notes, centerlines, hatching, and outlines on their own layers.
Control color, line weight, line style, and print visibility per layer.
Example: DIM layer black at 0.25mm, NOTE layer blue at 0.18mm, HIDDEN layer gray dashed.

Tip On PDF output, layers are preserved as PDF Layers, so recipients can toggle visibility per layer in Acrobat.

10. Drawing Finalization Best Practices

Standardize the Sheet Format at the company level. Align the logo, title block, revision block, and note text.
Use Layers. Separate dimensions, notes, centerlines, and hatching onto layers to control colors and line weights collectively.
Lock drawing views. If a view is moved by accident, the dimension layout falls apart. Right-click the view → Lock View Position.
Tangent Edges set to Visible by default are visually noisy. Change the drawing default to Removed or With Font (thin dashed).
Do not trust Auto-dimensioning. Auto dimensioning often misses critical dimensions. Manually review every dimension before release.
Automate the Revision Table. Wire up PDM Workflow Transitions so that a revision change automatically adds a row to the drawing's Revision Table.
Check anchor points before PDF output. If the anchor points for Balloons, BOMs, or Revision Tables have drifted off the sheet, the tables will print broken.

11. eDrawings — Lightweight Format for External Sharing

The official viewer that lets customers, suppliers, and sales check 3D models and drawings without SolidWorks installed. Free, with support for Windows/macOS/iOS/Android.

File formats:

.eprt — Part eDrawing.
.easm — Assembly eDrawing.
.edrw — Drawing eDrawing.

Features:

eDrawings Viewer (free): measurement, section, background change, Exploded View playback.
eDrawings Professional (paid): markup/annotation, animation recording, STL/3MF/AR export.

From SolidWorks, export via File → Publish to eDrawings; at that point you can set a password, expiration date, and whether measuring is allowed to protect IP. Commonly used for sharing sample files with suppliers for quoting.

Tip Sharing as eDrawings instead of STEP cuts file size to 1/5–1/10 while preserving dimensions and annotations. Optimal for design-review sharing.

12. xDesign and 3DEXPERIENCE Works

Dassault Systèmes's recent push is a browser-based CAD workflow, and increasingly it runs alongside traditional desktop SolidWorks.

xDesign: Runs in Chrome/Edge/Safari with no installation. Partial iPad support. AI-based auto Mate suggestions; can be used in both History-free and Parametric modes.
3DEXPERIENCE Works: Cloud platform. Syncs with desktop SolidWorks and lets you add Simulation, Manufacturing, and AI Copilot modules.
AR/VR integration: Review models placed in real space via Apple Vision Pro, Microsoft HoloLens, or iOS eDrawings AR mode.

For Korean SMBs in manufacturing, these are not the day-to-day primary tools yet, but the eDrawings + xDesign combination is practical for remote reviews and sales demos.

13. Common Mistakes and Check Points

Symptom	Cause	Remedy
Drawing doesn't reflect model changes	Reference-file path changed, files moved	`File → Find References` or PDM Check-In
Duplicate Model Items dimensions	Same feature dimension auto-placed in multiple views	Hide or delete the unwanted dimensions
Auto Balloons land outside the view	Number pattern too wide for the view scale	Realign with Magnetic Lines, enlarge the view
Blurry PDF quality	DraftSight default DPI too low	`Print → Options → High Quality` + 300 DPI
Hangul notes appear garbled	Template font doesn't support Hangul	Unify drawing Note font to Malgun Gothic or Nanum Gothic

Field Checklist

.slddrt Sheet Format standardized as the company format
Drafting Standard (ISO/ANSI/KS) consistent across drawings
Model Items dimensions not mixed up with Smart Dimensions
All necessary views present (Section/Detail/Broken as required), scales annotated correctly
Hole Callouts match the Hole Wizard source
GD&T symbols and datums align with quality-inspection methods
BOM Part Number driven by a Custom Property (not dependent on filenames)
Balloons aligned with Magnetic Lines
Lock View Position applied to every view
Revision Table wired into the Workflow
$PRPSHEET links in the title block are intact
PDF output tested at 300 DPI