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Line and Centerline

Sketches straight lines, and centerlines (construction lines) for revolve axes, mirror lines and layout.

Sketch tab > Line or Centerline (on the split button with Spline), or press L for Line. In the graphics area, right-click > Line also starts it.

A line chain being drawn, the cursor beside the "Midpoint, Horizontal" label with the preview segment snapped level.

Drawing Lines

  1. Click Line.
  2. Click the start point.
  3. Click the end of each segment. Each segment starts where the last one ended.
  4. End the chain: press Esc, double-click, or click the first point of the chain to close it. Clicking the loose end of another curve joins it and ends the chain too; a point where curves already meet, a midpoint or a point on a curve does not.

Press Esc again to return to the Select tool. Pressing and dragging from the start point to the end, then releasing, draws one line and ends the chain.

Centerline is drawn the same way, but each centerline is one segment: after its end point the next click starts a new one. Centerlines are drawn dashed and are construction geometry, so they are not part of profiles.

Automatic Relations

As the cursor moves, a label beside it names the relation the click adds:

Label Relation added
Coincident The point is shared with the existing sketch point. On the origin, a new point Coincident with it
Midpoint Midpoint of the sketch line
On line, On circle Coincident with the line, circle or arc
Horizontal, Vertical The segment is Horizontal or Vertical (Line and Centerline only)
Coincident (model) Coincident with a reference point at the model vertex
Midpoint (model edge), On edge (model) The model edge is projected into the sketch as reference geometry and the point is related to it
Center (model) Coincident with a reference point at the model circle's center
Coincident (other sketch) Coincident with a reference point at the other sketch's point

Relations to model edges and other sketches follow them when they change. The dashed blue inference lines line the cursor up with the X or Y of sketch points, model vertices and circle centers. A point placed on one is Vertical or Horizontal with the point it lines up with.

The other drawing tools snap the same way where they place a point of the new entity; each page says which.

Sketch Page

While the tool is active, the Sketch page shows the sketch's Status (Under Defined, Fully Defined or Over Defined) and the Tools, Model Edges and Pictures sections.

Select a line (with the Select tool) to show its relations and options:

Selected Entities
The selected items, by name (Line1, Centerline2).
Add Relations
The relations the selection can take. See Relations.
Existing Relations
The relations on the selection, each with a delete button.
For construction
Makes the line construction geometry. A construction line is a centerline.
Fix, Float
Fix holds the line's endpoints in place; Float releases them.
Delete
Deletes the selection.

Select one endpoint instead to set its X and Y under Parameters. Drag a line or its endpoints to move it within its relations.

See Also