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3D sketches

This is the reference page. If you are new to 3D sketching, start with Introduction to 3D sketching.

A normal sketch is flat: it lies on a plane or a face. A 3D sketch is not: its points have three coordinates, so it can run in any direction. It has no profile and cannot be extruded. It is made to be a path, for example for a sweep along a curve that bends in all three directions, like a handrail, a hose or a wire.

Quick start

  1. Choose 3D Sketch (Home tab, Sketch group, or command search). The tool opens in the left panel.
  2. Pick a mode (Line, Arc, Spline, Control spline or Points) and the Work plane to draw on.
  3. Click in the 3D view to place points. Each click lands where your pointer meets the work plane. To go off the plane, raise Height above plane or type X, Y and Z under Add by coordinates.
  4. Press Enter or Create to finish. Esc drops the chain you are drawing and a second Esc cancels the tool.

The keys the tool uses are:

KeyWhat it does
EnterFinish: the 3D sketch is added to the part.
EscDrop the chain being drawn; press again to cancel the tool.
Backspace or DeleteRemove the selected point (not while you are typing in a field).
Ctrl+Z / Cmd+ZStep back through the tool (the last point), not through the part.
Shift+click on a pointStart a new chain from an existing point.

The tool has no axis keys or gizmo: to move a point along the third direction, type its coordinate.

Drawing one

Choose 3D Sketch on the Home tab, in the Sketch group (on a phone, on the Sketch tab of the tools sheet), or search for “3D Sketch” in the command search. The tool opens in the left panel and takes over the 3D view.

Pick what to draw:

ModeWhat it makes
LineA polyline: click the corners. Click the last point again, or End chain, to stop; click the first point to close it.
ArcClick the start, a point on the arc, then the end. An arc of more than half a turn is made of several arcs that join up.
SplineA smooth curve that passes through every point you click. End chain stops it; clicking the first point again closes it.
Control splineA curve pulled towards the points but not through them. Set its Degree (3 by default; fewer points give a lower degree).
PointsSingle points.

Draw on the Work plane: Ground (the plane of the grid), Front, Top, Right, or any plane of the part. A plane you selected in the feature tree is the starting choice. Each click lands where your pointer meets the work plane.

Lifting points off the plane

  • Height above plane moves the work plane along its normal: set it to 40 and the next clicks land 40 mm above the ground. Change it between clicks to build a curve that rises and falls.
  • Under Add by coordinates, type X, Y and Z and press Add (or Enter): the point goes there, wherever it is.
  • Every point is in the Points list with its three coordinates. Type in a field to move it.

Snapping

With Snap to model and sketch points on, a click near one of these snaps to it, in space, ignoring the work plane:

  • a corner of the model (the end of an edge) and the middle of an edge;
  • a point of another sketch, flat or 3D;
  • a point you have already placed in this sketch (the click then reuses it, so lines and curves join).

A yellow cross shows where a click will land on the plane; a green cross shows a snap.

Editing while you draw

  • Drag a diamond to move that point in the work plane. For the third direction, type its coordinate.
  • Hover a diamond and it brightens and grows slightly. Click it to select it: the diamond turns red and its row in the list is highlighted (clicking a row selects the diamond too). The click area is larger than the drawn diamond, and larger again on a touch screen.
  • While you draw a chain, a click on an existing point does not select it: it joins the chain there, so the line or spline continues through that point, a click on the chain’s first point closes the outline, and a click on the last point ends the chain. Shift+click an existing point with no chain under way starts a new chain from it. Placing a new point clears the selection.
  • Select a point (click its diamond or its row) and press Backspace or Delete, or press × in the list, to remove it. A polyline closes up over the gap; a spline just loses that point.
  • Undo point removes the last point of the chain you are drawing. Ctrl+Z (Cmd+Z) steps back through the tool, not through the part.
  • Enter or Create finishes: one 3D sketch feature is added, as one undo step. Esc drops the chain you are drawing, and a second Esc cancels the tool.

Double-click the 3D sketch in the feature tree to open it again, with the same tools, and press Update. It is hidden, shown and suppressed like any other sketch, and drawn as a teal curve (the Curves display layer).

Sweeping along a 3D sketch

The kernel sweeps along a 3D sketch that holds exactly one spline (and nothing but points). A polyline or arcs in a 3D sketch are fine for reference, but cannot be a sweep path; the Sweep editor does not list them.

The introduction walks through this step by step with pictures. In short, a pipe along a curve:

  1. Open 3D Sketch, keep Spline, and click four or five points. Lift some of them with Height above plane. Leave Also add a plane normal to the start ticked, and press Create. You now have the 3D sketch and a Plane at its start, square to the curve.
  2. Select that plane in the tree and choose Sketch. Draw a circle (or any closed outline) around the origin and finish the sketch.
  3. Run Sweep (Home tab, Create group, in the list of the Loft button; Shift+W; or the command search). Profile is the new sketch; Path (open) offers the 3D sketch. Confirm.

The same path list is used by Path pattern.

What cannot use a 3D sketch

Guide curves of a sweep or loft, loft sections, Project curve and Rib take curves of flat sketches only; they do not list 3D sketches.

Not in the tool

The constraint solver for 3D sketches is in the kernel, but the tool does not offer constraints: you place and move points directly. Constraints already in a 3D sketch (for example from an import) are kept when you edit it, except ones that refer to a point you delete.

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