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.

Drawing Lines¶
- Click Line.
- Click the start point.
- Click the end of each segment. Each segment starts where the last one ended.
- 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.