Overview#
The Line and Arc tools are the workhorses of Fusion sketching. Nearly every outline that is not a rectangle or circle is built from connected lines and arcs, and even rectangles and slots are just convenient shortcuts for common line-and-arc arrangements. This page covers the Line tool (including its built-in tangent-arc behavior), the three Arc tools, and the Point tool, along with the numeric-entry techniques that let you draw accurately without placing every dimension afterward.
All of these tools live on the Sketch contextual tab, in the Create panel, and are available only inside an active sketch. This page also covers the Midpoint Line tool.
Where to find it#
| Tool | Location |
|---|---|
| Line | Sketch > Create > Line |
| Midpoint Line | Sketch > Create > Midpoint Line |
| 3-Point Arc | Sketch > Create > Arc > 3-Point Arc |
| Center Point Arc | Sketch > Create > Arc > Center Point Arc |
| Tangent Arc | Sketch > Create > Arc > Tangent Arc |
| Point | Sketch > Create > Point |
Press S to search any tool by name. While a line or arc tool is active you can switch between its types in the Feature Options section of the Sketch Palette.
Note: not confirmed in Autodesk's documentation: single-key shortcuts for these tools. Autodesk's sketch help documents only S (toolbox search) and D (Sketch Dimension). Keys such as L for Line are common defaults in practice; check yours under Preferences.
Step by step: drawing lines#
- Choose Line from the Create panel (the L key is a commonly used default, not listed in the help).
- Click once in the canvas to place the start point. If you snap to an existing point, the logical constraints (such as Coincident) are added automatically.
- Specify the length and angle of the segment: either click to place the second point, or enter the length and angle values and then place the point.
- Continue placing points to add more connected segments.
- To close a profile, click the start point.
- Click the Check icon, or press Enter, to complete the tool.
Typed entry rules#
You can enter the length and angle values instead of clicking, which gives an exactly sized segment. The Tab key switches between the length and angle fields in the polygon, ellipse and slot tools, and works the same way here. A segment you merely click into place has no dimension and is under-defined.
Note: not confirmed in Autodesk's documentation: whether typed values also create driving dimensions, and the lock icon shown after Tab. Check the dimension appears in your sketch before relying on it. Expressions in dimensions are covered on the dimensions page.
Switching to a tangent arc while using Line#
While the Line tool is active, pause over an end point, then click and drag to create an arc segment that is tangent to the previous line segment. Move the mouse to the opposite side of the line segment to flip the direction of the arc. You can specify a radius before you create additional segments. This lets you draw an outline of alternating straight and curved sections without leaving the Line tool.
Inference and snapping#
As you move the cursor, object snap symbols display near the geometry when you snap to the sketch grid or other geometry in the design. If you snap to a specific point, the logical constraints are automatically added to the sketch. Typical inferences are Horizontal/Vertical, Coincident, Midpoint, Perpendicular, Parallel and Tangent.
If an unwanted constraint appears, undo or delete its badge afterwards.
Note: not confirmed in Autodesk's documentation: holding Ctrl to suppress inference, or a Constraint Settings list in the Sketch Palette.
Arcs#
Fusion has three arc tools; while one is active, the Sketch Palette Feature Options let you switch between them:
3-Point Arc#
Click to place the first end point, specify a distance and click the second end point, then click a third point that lies along the arc. The arc passes through all three points. Use it when you know where the arc starts, ends, and roughly where it passes.
Tangent Arc#
Click the first end point so that it coincides with the sketch geometry that will receive the tangent constraint, then click the second point or specify a radius. Use it for smooth transitions and organic outlines.
Center Point Arc#
Click the center point, click the first end point (which also sets the radius), then click the second end point or specify an angle value. Use this when the center and radius are the important design values, for example a bolt circle or a hinge radius.
Arc dimensions#
An arc can be driven by radius, by its end points, or by its swept angle. With the Sketch Dimension tool (D), click the arc to dimension its radius or select its end points for a distance. See the dimensions page for the full selection rules.
Points#
The Point tool (Create > Point) places sketch points: click in the canvas (snapping to the grid or existing geometry), then press Enter. Points are useful as reference geometry to constrain other geometry, and as location markers; a point can be dimensioned from the origin or from edges so that a position is edited by changing one dimension. Points are never part of a profile.
Note: not confirmed in Autodesk's documentation (sketch help): that the Hole command accepts sketch points as placement positions.
Options reference#
| Option | What it does | Notes/default |
|---|---|---|
| Length and angle input | Sets the segment length and angle | Enter values instead of clicking the second point |
| Chaining | Each new segment starts where the last ended | Click the start point to close; Check icon or Enter completes |
| Tangent from endpoint | Pause over an end point, click and drag to create a tangent arc segment | Move to the opposite side to flip the arc |
| Midpoint Line | Click the midpoint, then place the end; the line is symmetric about the midpoint | |
| 3-Point Arc | Two end points and a point along the arc | Good when the arc must pass through a known point |
| Tangent Arc | First end point coincides with existing geometry that receives the tangent | Second point or radius value |
| Center Point Arc | Center, first end point, second end point or angle | Radius is set by the first two clicks |
| Point | Places a reference point | Press Enter to finish |
| Linetype | Normal or Construction | Set in the Sketch Palette |
Tips and pitfalls#
Tip: Draw rough, then dimension. For quick outlines, click anywhere, then use D to dimension each segment. The shape snaps to the true values. It is often faster than typing every length as you draw, especially when you change your mind.
Tip: Enter length and angle values rather than clicking when you need an exact segment.
Tip: Start outlines on the origin or on a projected edge. The first point of a sketch is the one with no anchor; making it coincident to the origin gives the solver a head start.
Warning: Do not close a profile with a near-miss click. If the last click lands a pixel beside the first point rather than on it, you have a gap that is invisible at normal zoom and the profile will not shade. Look for the coincident dot or run the profile check described in the troubleshooting page.
Warning: The Tangent Arc tool needs its first point on existing sketch geometry to receive the tangent constraint. If the result is not tangent, check where you started.
Practice exercise#
Draw an L-shaped bracket outline with a rounded inside corner using only the Line and Tangent Arc tools:
- Start at the origin and draw: 60 mm right, 20 mm up, 40 mm left, 40 mm up, 20 mm left, and back down to the origin, entering length and angle values for each segment.
- Replace the inside corner with a tangent arc: delete the two segments meeting at that corner, then draw a Tangent Arc from one remaining endpoint to the other.
- Dimension the arc radius to 8 mm.
- Finish the sketch and extrude the profile 5 mm.
Expected result: a closed profile that shades blue and extrudes into a bracket with a smooth inside curve. Edit the radius and observe the corner change.
Related#
- Rectangles, circles, polygons, ellipses, and slots (02-sketching/shapes)
- Constraints (02-sketching/constraints)
- Dimensions (02-sketching/dimensions)
- Trim, extend, fillet, and offset (02-sketching/modify-tools)