Drafting Workbench - Practical Guide: Drawings, Dimensions, and GD&T

CATIA · Drafting

Overview

Drafting is the workbench that turns 3D models into 2D production drawings. This page covers Sheet and View setup, Section / Detail views, dimensions, annotations, GD&T (FTA) integration, and the day-to-day workflow that keeps drawings automatically in sync with 3D changes.

For Assembly and Part Design itself, refer to pages 02 and 03 respectively.

1. Starting a Drafting Session and Standard Setup

Path: File → New → Drawing, or Start → Mechanical Design → Drafting.

Decide four things up front in the dialog.

Item	Options	Field tip
Standard	ISO / ANSI / JIS / ASME / GB / DIN	ISO is the default for Korean primes; ASME for US exports
Sheet Style	A0 – A5, Letter, Legal, Custom	A Custom template carrying the company's title block is strongly recommended
Scale	1:1, 1:2, 2:1 …	Large parts at 1:2 / 1:5, precision parts at 2:1 / 5:1
Orientation	Landscape / Portrait	Pick to match your title-block layout

Tip Build a .CATDrawing template once, embedding the company logo, title block, and drawing-number convention, and register it at Tools → Standards → Drafting. Every team member then starts from the same form each time they click New. Without a template, every drawing diverges slightly block by block and quality control collapses.

Note Changing the Standard mid-project is heavily restricted. Some dimension styles are bound to the Standard, and swapping it later can break layouts — lock it in at project kickoff.

2. View Creation System

Insert → Views menu or the View toolbar.

Front View — base front view created by picking a starting face in 3D
Projection View — left / right / top / bottom / isometric projections from the Front (watch ISO 1st-angle vs. 3rd-angle)
Auxiliary View — projected normal to a tilted reference face. Essential for inclined holes or angled flanges.
Isometric View — isometric auxiliary
Section View / Section Cut — sections. Offset Section (stepped) and Aligned Section (rotational unfold) are both supported.
Detail View / Detail View Profile — enlarge a circular or free-form region
Clipping View — shows only a cropped region of a View
Broken View — collapses the middle of long shafts or beams
Broken-out Section — partial section (local internal exposure)
Unfolding View — Sheet Metal unfolded view
View From 3D — carries over 3D Annotation such as FTA as-is

Tip If a Section comes out reversed, right-click the Section Line → Reverse Direction. Label suffixes (A-A, B-B) can also be edited manually from Properties.

Note ISO (1st angle) and ANSI (3rd angle) arrange projections oppositely. When exchanging drawings with overseas partners, the Sheet's Projection Method must be stamped on the document to avoid confusion.

3. Section and Detail in Practice

3.1 Section Construction

A Section Line can be a polyline with two or more points; each kink turns it into an Offset Section. Hatching is auto-filled in the section, and material-specific hatch patterns are changed at Properties → Pattern.

Aligned Section — rotational-unfold section for symmetric rotating parts (e.g., gear-web holes)
3D Section Callout — pulls a Section Plane annotated in 3D straight into drafting

3.2 Repositioning a Detail View

Even after creation, you can drag the Detail Profile (circular boundary) on the parent View to rebound the range. The Profile itself can also be moved to another View (especially flexible in 3DEXPERIENCE).

Tip Instead of the Detail circle, use Detail View Profile and define the boundary with a sketch when you need a free-form enlargement. Handy for non-circular close-ups.

4. Dimensions

The automatic dimension tool infers distance / angle / radius based on the type of the selected edge or face.

Tool	Use
Dimension	General-purpose, auto-infers type
Chained Dimension	Chained dimensioning (end-to-end)
Cumulated Dimension	Cumulative dimensioning from a datum
Stacked Dimension	One datum, multiple extension lines
Length/Distance	Linear distance
Angle	Angle
Radius/Diameter	Radius / diameter
Chamfer	Single-line chamfer callout
Thread	Automatic thread-spec callout
Coordinate	Coordinate dimension table

Tip With a dimension selected, right-click → Properties → Value tab to edit Tolerance, Prefix, Suffix, and Fake Value.

Fake Value is used to decouple the drawing value from the real 3D dimension — for example, to show shrinkage compensation on mold drawings. Overusing it is the root cause of 3D-2D mismatches, so always log the reason in the Notes.

Note Accumulating tolerances with Chained Dimensions lets the end-of-chain tolerance blow up. Functional dimensions are safer driven Cumulated, directly from a Datum.

5. Annotations

Text / Text with Leader — plain text, with optional leader
Balloon — balloon callout (item number), auto-linked to the BOM Table
Datum Feature / Datum Target — datums
Geometrical Tolerance — GD&T frame (see 6.6)
Roughness — surface-finish symbol (Ra, Rz, Rmax)
Weld — welding symbol (Weld Design annotations can be auto-imported)
Table — BOM / revision history / other tables

Tip Beyond manual placement, the Generate Balloons command lets you batch-assign balloons to every part in the BOM. A huge time saver on large assembly drawings.

6. GD&T and FTA Integration

6.1 FTA (Functional Tolerancing & Annotation) Flow

Under Start → Mechanical Design → Functional Tolerancing & Annotation, apply tolerances and datums directly to the 3D model. Then bring them into Drafting via View from 3D and the 3D annotations land on the 2D drawing as-is.

6.2 Geometric Tolerance Symbols

Symbol	Meaning	Category
—	Straightness	Form
⏥	Flatness	Form
○	Circularity	Form
⌭	Cylindricity	Form
∥	Parallelism	Orientation
⊥	Perpendicularity	Orientation
∠	Angularity	Orientation
⌖	Position	Location
◎	Concentricity	Location
⌯	Symmetry	Location
⌓	Profile of Line / Surface	Profile
↗	Circular Runout	Runout
⌰	Total Runout	Runout

6.3 Setup Tips

Path: Tools → Options → Mechanical Design → Functional Tolerancing and Annotation → Manipulators.

Enabling every Dimension Manipulator entry makes leader movement and rotation free. The default configuration ships with some disabled, which often makes frames feel frozen in place.

Note GD&T is not drawing decoration. Datum precedence (A|B|C) and the choice of MMC / LMC directly change inspection methods and the allowable envelope. Imprecise intent leads to inspection disputes at mass production.

7. Text Style and Sheet Management

7.1 Text Style / Dimension Style

At Tools → Standards → Drafting, you can edit styles such as fonts, character height, arrow size, and extension-line gaps. Since they are XML-based, the efficient model is for IT to author a company-standard file once and distribute it.

7.2 Sheet Structure

Main Sheet — the actual working area
Background View — fixed layer holding the title block, company logo, and frame. Switch via Edit → Background View.
Working View — the active layer carrying dimensions and views. Return via Edit → Working Views.

Tip Using Link to Excel in the Background View to pull certain title-block cells (drawing number, revision, author) from Excel centralizes drawing metadata across the whole team.

7.3 Duplicating a Sheet

Right-click the Sheet tab → Duplicate. Copies existing Views and dimensions wholesale. Handy for stamping out similar drawings.

8. Handling 3D Changes and Drawing Updates

If a drawing does not reflect a 3D edit automatically, check the following.

Verify Tools → Options → Mechanical Design → Drafting → General → Synchronize Views during Update is ticked
Run Edit → Update, or Update All Views on the toolbar
Review Drafting-to-3D links at Edit → Links. If a Part name or path changed, reconnect with Replace
If dimensions follow the "Driving Dimension" scheme tied to 3D edges, they update automatically when the 3D value changes

Note Even when the whole-drawing update succeeds, annotations (text, GD&T) can become orphans when the 3D structure changes significantly. After a large 3D change, make eyes-on review of the entire drawing part of the process.

9. Drafting Practical Tips Bundle

Hide View Frames — always hide View borders before printing
Dress-up — apply centerlines, thread lines, and arrows manually via the Dress-up tools
Multi-View Projection — when FTA annotations exist on the 3D, all required views can be generated automatically
BOM Automation — Insert → Generation → Bill of Material → pick a template → auto-updates on refresh
PDF Export — File → Print → Microsoft Print to PDF, or stay on ISO-A3 settings
No-Computed-Dimensions Rule — overuse of Fake Value is a major source of inspection mismatch

10. Drawing Layers and Overload

Drawings support layer and visibility management just like Parts and Assemblies.

Layer Filter — Tools → Visualization Filters. Show / print specific layers only.
Graphic Properties — per-element color, line type, and line weight
Overload Properties — bulk overrides at the View level

Tip Defining a company-standard layer set (e.g., 1 = visible edge, 2 = hidden edge, 5 = center line, 9 = dimensions) keeps output uniform even when different engineers draw it.

Note Rather than attaching colors directly to elements, driving them via layer-based Graphic Properties is far easier to maintain.

11. Title Blocks and Property Linking

Place the company-standard title block in the Background View and auto-link cells to Part / Product Properties to reduce errors.

Insert → Drawing → Link to 3D Properties — bind Part Number, Description, Revision, etc., to title-block text
Link to Excel — manage title-block cells from Excel
Insert → Text → Text With Leader — standardize notes on text-with-leader

Tip Rather than typing the approver / author / checker names manually, exposing them as Environment Parameters of the .CATDrawing lets each team member enter their name only once.

12. Drawing Output and PDF Quality

Page Setup — always pre-verify Sheet Size, Orientation, and Margin
Print to File — 300 dpi or higher is recommended for PDF
Line Thickness Table — map at Tools → Standards → Drafting → Thickness Table to tune actual printed weights
Gray / Color — tick Gray Conversion so light colors do not fade out on black-and-white printers

Note When sending drawing PDFs to overseas partners, unflattened annotations (comments / markup) can leak sensitive information. Always flatten PDFs for delivery.

13. Frequent Drafting Issues

Symptom	Cause	Fix
Drawing not updated after 3D change	Synchronize option off	Tools → Options → Drafting → tick Synchronize
Dimension shows as "?"	Referenced edge deleted	Edit → Links, or recreate the dimension
Section hatch direction wrong	Material pattern mismatch	Properties → Pattern, reassign
Balloon numbers don't match BOM	Manually edited fixed numbers	Regenerate via Generate Balloons
GD&T frame not editable	Bound to 3D FTA source	Edit in FTA and regenerate the View
Title-block text missing	Broken link	Reconnect via Link to 3D Properties

Tip More than 70% of drawing-quality issues trace back to "link sync after a 3D change." Make Edit → Links inspection a regular routine.

14. Format Exchange and Partner Handoff

When sending drawings outside, understand the quirks of each format.

PDF — best viewer compatibility. Flatten before delivery.
DWG / DXF — AutoCAD-compatible. Some dimension / annotation styles may drop.
TIFF / PNG — high-resolution images, suited for scans
3D PDF — 3D model + drawing combined. Convenient for partner review but large in size.

Tip When exporting to DWG, tune Polyline / Spline conversion and Text Mapping at Tools → Options → Compatibility → DXF to make the 2D layout land correctly.

Note Exporting your in-house dimension styles and layer scheme straight to DWG frequently makes colors and line weights tangle in the partner's environment. Always vet one test DWG with the partner before the real handoff.

15. Real-World Working Tips

Five-pack of drawing templates — build A4 / A3 / A2 / A1 / A0 templates and register them. Users only pick when adding a Sheet.
Revision control — keep the Revision Block on a separate Sheet and add a row per change
Standardized Notes — save shared notes like "General tolerance: ISO 2768-mK", "Surface roughness: Ra 3.2", and "Material: STEEL S45C" as a Catalog
Copy dimensions — Ctrl+drag to copy dimensions while preserving style
Quick View Create — save the Front / Top / Right Planes already declared in 3D Part as Named Views, and pull them directly into Drafting via View From 3D
Assembly Drawing — for exploded views, first build a Product Scene or Enhanced Scene, then bring it into Drafting — that flow is the most stable
Welding Symbol Automation — embed weld info on the 3D with Weld Design and let Drafting extract it automatically

Field Checklist

Is the company-standard Drafting Sheet template registered?
Is the Projection Method (1st / 3rd angle) stated on the sheet?
Do Dimension Style and Text Style match the team standard?
Do Section direction and labels match the actual inspection intent?
Does the datum precedence in GD&T frames match design intent?
Is Synchronize Views during Update turned on for handling 3D changes?
Did you hide View Frames before the PDF export?
Were BOM balloons batch-matched via Generate Balloons?
Have the 3D FTA annotations all propagated into the 2D drawing?
If a Fake Value is used, is the reason recorded in Notes?