Annotations, Text, and Notes

Overview#

Beyond dimensions and symbols, a drawing carries notes: general notes ("Break all sharp edges 0.3 max"), material and finish callouts, thread and hole notes, revision information, and view labels. Fusion's drawing annotations also include geometric helpers such as centerlines, center marks, and edge extensions.

Notes are plain text unless generated from the model (hole notes, title block fields). Put manufacturing requirements that apply to the whole part in a notes block, and feature-specific information near the feature.

Where to find it#

Drawing workspace toolbar:

• Geometry panel: Center Line, Center Mark, Center Mark Pattern, Edge Extension, Create Sketch.
• Text panel: Text, Note (creates a leader, hole and thread, or bend note automatically from what you pick), Leader, Hole and Thread Note, Bend Note.
• Create > Create Sketch for sheet-level 2D linework not tied to the model. Autodesk's list has no Chamfer Note command.

Step by step: text and leaders#

1. Choose Text.
2. Click to place opposite corners of the text box, then type and format the text: Font, Height, Bold, Italic, Underline, bulleted, numbered and lettered lists, Justification and Symbols (from the Symbols flyout).
3. Click anywhere on the sheet or click Close to finish.
4. For a leader note, choose Leader, click the feature, click where the text goes, and type.
5. To insert model data, choose a Type, Source and property in the text dialog (Insert Property); model properties and parameters can go into leaders, text, custom tables and dimensions.

Text can be moved by dragging, and edited by double-clicking.

Step by step: Hole/Thread Note#

1. Choose Text > Hole and Thread Note.
2. Click the edge of a hole or thread feature, then click to place the leader and text. The text populates automatically from the feature.
3. Click further features to add more notes, then click Close.
4. Double-click the text to edit it (for example to add a count such as 4X).

Autodesk states you can also make thread notes for threads added to extruded cuts (internal) or extruded circular profiles (external), not only to Hole-command features. If you edit or delete the generated text and fields, you must recreate the note to restore them. Moving the arrowhead disassociates the note from its feature.

Step by step: centerlines and center marks#

1. Choose Geometry > Center Mark and click a circle or arc edge. A cross appears at the center.
2. Choose Center Mark Pattern and click holes to annotate circular geometry as a pattern.
3. Choose Center Line and select two lines or straight edges to create a center line between them.
4. Select a center line and drag the grey arrow grips to lengthen or shorten it.

You can also generate center marks and center lines for whole classes of holes in the Drawing View dialog (Automated Center Marks and Center Lines).

Sheet-level sketches#

Create > Create Sketch enters a sketch environment with Geometry, Constraints, Modify, Text and Measure tools. Clicking a drawing view creates a View Sketch, associative to that view (it moves and scales with it); clicking outside any view creates an independent sketch. A view sketch does not change the 3D model. Use sketches for:

• Custom border elements
• Simple diagrams or schematic notes
• Material callout boxes

Revision clouds and markers have their own commands (see the tables page).

General notes block#

A typical notes block, placed at the lower left or above the title block:

1. UNLESS OTHERWISE SPECIFIED: DIMENSIONS ARE IN MM.
2. GENERAL TOLERANCES ISO 2768-m.
3. BREAK ALL SHARP EDGES 0.3 MAX.
4. MATERIAL: 6061-T6 ALUMINUM.
5. FINISH: BLACK ANODIZE, TYPE II.
6. REMOVE BURRS.
7. DO NOT SCALE DRAWING.

Put this in your template as a text object so it appears on every drawing, and edit per part.

View labels and sheet information#

• View labels show the name, identifier and scale of section and detail views.
• Sheet information (sheet number of total) appears in the title block and updates automatically.
• Revision table: Tables > Revision History logs revisions and drives the title block REV attribute.

Options reference#

Tips and pitfalls#

Tip: Write notes in imperative, unambiguous language. "Deburr all edges" beats "edges should be deburred".

Tip: Put repeated notes in the template to avoid retyping and ensure consistency.

Tip: Use leader notes with an arrow to the feature, rather than relying on location, so the note cannot be misassociated.

Warning: Typed text is not linked to the model. A note that says "6061-T6" will not change if the material changes in the design. Use Insert Property where possible.

Warning: Hole notes reflect the model at the time of generation; after a model change click Get Latest and check disassociated notes (Annotation Monitor badge, Reassociate).

Warning: Do not hide vital information inside the title block. Machinists look for notes near the views.

A note schema that scales#

Every note on a drawing belongs to one of four categories, and keeping them separate stops the sheet from becoming a pile of text.

Numbered general notes can be referenced from feature notes with a flag, for example "SEE NOTE 4" or a note number in a small circle or triangle. Do not repeat the text of the note in several places.

Hole note content in detail#

The Hole and Thread Note populates its text from the hole or thread feature, so a tapped hole gives a thread designation and depth (the exact format is not shown in Autodesk's help; check your own result). Editing the note lets you add the count ("4X") or remove parts, but hiding the depth does not change the model. If you cannot restore the generated text, recreate the note.

Worked example: text sizing#

Text should be readable at the printed size. A common minimum for drawing text is 2.5 mm height for notes and 3.5 mm for titles; on an A3 sheet printed to A4 (a reduction of about 70 percent) 2.5 mm becomes 1.75 mm, which is hard to read. If a drawing will be photocopied or viewed on a phone, choose 3.5 mm for notes. As a quick check, export a PDF, print it at A4 and read the smallest note at arm's length. Line count matters too: a notes block of 12 lines at 3.5 mm with 1.5 mm line gaps is about 60 mm tall, which fits above a title block but not next to a crowded view.

Centerlines and center marks: what to expect#

Center marks mark the center of circles and arcs; center lines run through axes of cylinders and symmetric features. For a bolt circle, a Centermark Pattern adds a circular center line through all the holes, plus a cross at each. Extend centerlines slightly beyond the outline (general practice, 2 to 3 mm), and keep them out of dimensioning spaces by stopping them at the first extension line. The Drawing View dialog can also add center marks and center lines automatically for selected hole types, which saves manual work on plates with dozens of holes.

Failure modes and fixes#

Workflow advice#

Write the notes block last, after the views and dimensions are stable, but build the skeleton in the template. Keep notes imperative, specific and measurable ("deburr edges 0.2 to 0.5", not "deburr"). Avoid duplicating information that the title block already has. For a drawing that will be revised, number each note and never reuse a deleted number; the revision table can then say "note 5 changed". For parts with long manufacturing instructions, a separate sheet of notes is better than an overcrowded view sheet.

Use sheet-level sketch geometry sparingly and only for things that are not model-related: revision clouds, a small flow diagram, a border cut-out. Anything that describes the part belongs in a model-linked view or annotation, so that it updates when the model does.

Practice exercise#

1. On the Bracket drawing add center marks to all holes and a centerline through the slot. Extend the slot centerline 3 mm beyond the outline.
2. Add a Hole/Thread Note to the two holes. Edit it to read "2X" and check that the diameter matches the model.
3. Create a notes block with five numbered notes: units, general tolerance ISO 2768-m, break edges 0.3 max, material, finish. Set the text height to 3.5 mm.
4. Add a leader note "DEBURR SLOT EDGES, SEE NOTE 3" pointing at the slot.
5. Change the material in the design, click Get Latest and see which text changed on its own. Then replace the typed material note with an Insert Property field.
6. Export to PDF, print at A4 and verify that the smallest text is readable at arm's length.
7. Expected result: all holes carry center marks, a model-derived 2X note, a clear numbered notes block, a cross-referenced leader note, and a material callout that updates when the design changes.

Related#

• Dimensions and tolerances
• GD&T and symbols
• Tables, parts lists, and balloons