GD&T and Drawing Symbols

Overview#

Geometric Dimensioning and Tolerancing (GD&T) communicates the allowed variation of form, orientation, location, and runout relative to datums. Fusion's Drawing workspace provides a Symbols panel with the annotation objects needed to write it: Surface Texture, Feature Control Frame, Datum Identifier, Welding, Taper and Slope, Edge Symbol and Sketch Symbol.

Fusion draws the symbols; it does not check that your GD&T is correct or inspect the model against it. You must know the rules. This page covers the tools and a concise primer; for rules, read ASME Y14.5 or the ISO GPS standards.

Where to find it#

Drawing workspace toolbar, Symbols panel:

• Surface Texture
• Feature Control Frame
• Datum Identifier
• Welding
• Taper and Slope
• Edge Symbol (edge processing and finishing requirements)
• Sketch Symbol (custom symbols, flag notes, inspection bubbles, custom balloons, ISO/DIN 5459 style datum target symbols)

There is no separate Datum Target command in Autodesk's help; use a sketch symbol for datum targets. Balloon lives in the Tables panel (see the tables page). Use the Text panel for notes. The drafting standard (ASME or ISO) defines each symbol's properties and the characters in the Symbol palette, so choose it before you create the drawing.

GD&T characteristics#

Under ASME Y14.5-2018, concentricity and symmetry were removed in favor of position and profile; ISO still defines them. Use those that your customer's standard allows.

Step by step: Feature Control Frame#

1. Choose Symbols > Feature Control Frame.
2. Select the edge of an object, or the text of a dimension or note. Frames can attach to notes and to linear, diameter, radius and angular dimensions.
3. For an edge, click the start point, then click to place the leader (a click adds a bend), and press Enter or click the check mark. If you picked dimension or note text, the frame is placed under it and moves with it.
4. In the Feature Control Frame dialog add tolerances and symbols: type your own alphanumeric characters or pick from the Symbol palette, whose characters are defined by the ASME or ISO standard.
5. Click OK.

For ISO drawings you can also create a surface identification leader: choose the edge, right-click for the marking menu and pick Surface. The frame stays perpendicular to the edge or its extension line. Fusion remembers the last-used settings; Reset clears them. Autodesk's help does not itemize modifiers, datum fields or composite frames, so look in the Symbol palette for what your standard offers.

Step by step: Datum Identifier#

1. Choose Symbols > Datum Identifier.
2. Select the edge of an object, click the start point (inside the edge for a straight leader, beyond it for a surface extension), then click the next point and press Enter or click the check mark.
3. Fusion auto-fills and auto-increments the identifier (A, then B, and so on); edit the Identifier field to change it. By general GD&T practice (not Autodesk guidance) avoid I, O, Q, S, X and Z as datum letters. With the ISO standard you can add a datum note and thread note.
4. Double-click an existing datum ID to edit it.

Step by step: Datum Target#

Datum targets define points, lines, or areas used to establish a datum on irregular surfaces such as castings. Autodesk's Symbols panel has no Datum Target command. Instead, the Sketch Symbol tool lets you create, insert and edit custom symbols with leaders and automatic alpha or numeric counters, which Autodesk gives as the way to make ISO/DIN 5459 style datum target symbols. Create the symbol once (Create a sketch symbol), then insert it where needed.

Surface Texture#

1. Choose Symbols > Surface Texture.
2. Select the edge of an object, then click the start point and next point (a click adds a bend). Surface textures can also attach to existing dimensions and feature control frames.
3. Press Enter or click the check mark, then in the Surface Texture dialog select the symbol type and add annotations. The options available depend on the drafting standard and the symbol type.
4. Click OK. On ISO drawings a surface identification leader (marking menu > Surface) is also available, and the Area field of the identifier switches between near and far side.

Autodesk's help does not list the individual roughness fields; check the dialog for what your standard offers.

Welding Symbols#

Symbols > Welding works like the other leader symbols: select an edge, place the leader, then fill in the Welding dialog. The options depend on the drafting standard and weld symbol type. Autodesk's Welding reference lists the supported standard revisions as AWS A2.4-1998, AWS A2.4-2012 and ISO 2553:2019 with ISO 4063:2009, and includes all-around, field weld, spacer, weld system and stagger properties depending on the revision. Taper and Slope and Edge Symbol have their own references.

Options reference#

Example: position of a hole pattern#

1. Dimension the hole diameter with a tolerance, such as 6.0 +0.1 / 0.
2. Dimension the hole location with basic dimensions from datum edges (boxed values). In the Dimension dialog use the Theoretically Exact representation.
3. Attach a feature control frame to the hole diameter dimension: Position | diameter 0.2 M | A | B.
4. Attach datum identifiers A and B to the plate's bottom face and left edge.

The plate is now toleranced for hole position relative to its primary and secondary datums.

Tips and pitfalls#

Tip: Choose datums that match how the part is located in its assembly or fixture. Datums are not decoration.

Tip: Use basic dimensions only with a position, profile, or angularity frame. A basic dimension with no frame is incomplete.

Tip: Keep feature control frames next to the feature, attached to the dimension or surface, not floating.

Warning: Fusion does not validate GD&T logic. A frame can be syntactically correct and meaningless. Review with someone familiar with Y14.5.

Warning: When you export to DWG, Datum ID, Feature Control Frame, and Surface Texture annotations are simplified, and dimensions lose associativity. Expect to re-check them in the receiving CAD program, or send a PDF for authoritative content.

Warning: Material condition modifiers (M, L) matter only when the feature is a feature of size. Applying them to a flat surface is an error.

Note: ASME and ISO use different symbols and rules (for example ISO uses envelope requirement and independence principle differently). Match the symbols to the standard chosen in your template.

What the tools are, per Autodesk#

Autodesk's "Geometric tolerancing symbols" help describes the Symbols panel and notes that you can attach feature control frames to model components and to existing dimensions, while datum IDs and surface textures attach to components, dimensions and feature control frames. After creation, a symbol stays associated with its object; if it becomes disassociated, use the Annotation Monitor badge and Reassociate. Fusion does not check GD&T logic.

Reading a feature control frame#

A frame is read left to right: characteristic, tolerance zone (with a diameter symbol if the zone is cylindrical, plus any material modifier), then up to three datum references in order of precedence. For example, the frame "Position | diameter 0.2 (M) | A | B | C" says: the hole axis must lie inside a cylinder of 0.2 mm diameter (at maximum material condition) whose position is located relative to datum A first, B second and C third. The order encodes the fixturing: the part sits on A (three contact points), is pushed against B (two points) and then against C (one point).

Worked example: a mounting plate#

A plate 100 x 60 x 8 mm with four 6 mm holes (6.0 +0.1 / 0) at 10 mm from the edges.

1. Datum A is the bottom face (the mounting surface); datum B is the long left edge; datum C is the short bottom edge.
2. Dimension hole positions as basic dimensions: 10, 90, 10 and 50 mm from the datum edges.
3. Attach the frame Position | diameter 0.2 (M) | A | B | C to the hole diameter dimension, with "4X" in front.
4. Because of the MMC modifier the hole's position tolerance can grow when the hole is larger than its smallest size: the smallest hole is 6.0, so at 6.1 the allowed position zone grows to 0.2 + 0.1 = 0.3 mm. This is the bonus tolerance, and it is the reason MMC is chosen for clearance holes.
5. Flatness of the mounting face: a frame with the flatness symbol and 0.05, attached to the surface with a leader, no datum references.

Check: the flatness value must be smaller than any size tolerance that the surface is controlling, otherwise it adds nothing.

Surface texture numbers#

As general guidance (not Autodesk data), on milled and turned parts typical callouts are Ra 3.2 (general machined), Ra 1.6 (bearing seats and sealing faces), Ra 0.8 (ground or fine-turned) and Ra 6.3 (rough machined, cosmetic). Metric drawings show micrometers; inch drawings show microinches (Ra 1.6 micrometers is about 63 microinches). Put the general default in the title block ("all surfaces Ra 3.2 unless noted") and use the symbol only on exceptions.

Failure modes and fixes#

Workflow advice#

Decide the datum scheme from the assembly, not from the drawing: which faces touch other parts, and in what order does the part get located? Sketch the scheme on paper. Then add datum identifiers, then basic dimensions, then frames, in that order, because each step depends on the previous. When in doubt, use fewer tolerances rather than more: every frame costs inspection time. A good rule is to tolerance only the functional features (mating holes, sealing faces, bearing seats) and leave the rest to general tolerances. Have a second person who knows the standard read the print before release, because Fusion will not validate logic.

Practice exercise#

1. On the Bracket drawing place datum identifier A on the bottom face and B on the left edge. Choose letters that avoid I, O, Q, S, X and Z.
2. Convert the hole position dimensions to basic dimensions (Theoretically Exact representation).
3. Attach Position | diameter 0.2 (M) | A | B to the holes with "2X". Calculate by hand the allowed position zone when the hole is at 6.1 mm (answer: 0.3 mm).
4. Attach Flatness 0.05 to the mounting face and Perpendicularity 0.1 | A to the left face.
5. Add a surface texture symbol Ra 1.6 to the mounting face and a general note "ALL OTHER SURFACES RA 3.2".
6. Export a PDF and a Simplified DWG and compare how the frames survive.
7. Expected result: two datums, three frames, a basic-dimensioned hole pattern, a surface finish callout, a hand-calculated bonus tolerance of 0.3 mm and a comparison showing simplified frames in the DWG.

Related#

• Dimensions and tolerances
• Annotations, text, and notes
• Export to PDF, DWG, and DXF