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Trim and Extend Entities

Trim Entities deletes the piece of a sketch entity between its intersections with other sketch entities. Extend Entities carries the end of a line or arc on to the next entity it meets.

Sketch tab > Trim Entities or Extend Entities (on one split button), or press T for Trim Entities.

Two crossing lines and a spline before and after trimming, with the removed pieces shown dashed in the before image.

Trimming

  1. Click Trim Entities.
  2. Select the piece to remove, or drag across several pieces. A gray line follows the pointer, and each piece it crosses is removed as it crosses it.
  3. Repeat for other pieces. Press Esc to return to Select.

Trim has no property panel page; the sketch's page stays up while it is active. Each click, and each drag, is one undo step (Ctrl+Z).

What Is Removed

The piece clicked runs from the nearest intersection on one side to the nearest on the other, or to the entity's end where there is no intersection on that side. Intersections are with lines, arcs, circles and splines; construction geometry does not cut.

Piece clicked Result
No intersection on either side The whole entity is deleted
An end piece The entity is shortened to the intersection
A middle piece The entity is split in two

Trim works on lines, arcs, circles, ellipses, parabolas, conics and splines.

A trimmed circle becomes an arc, and a trimmed full ellipse a partial ellipse. It stays the same entity, so its relations and its radius or diameter dimension stay. A circle or ellipse needs two intersections to be trimmed; with fewer, it is deleted.

Relations Added

Each new end is tied to the entity that cut it, so it stays there as the sketch changes:

  • Where the cut is at that entity's end point, the two points are merged (coincident).
  • Otherwise the end is kept on that line, arc or circle.

A line split in two stays one line: the pieces get a Collinear relation, and a Horizontal or Vertical relation on the original is copied to the second piece. Dimensions on the trimmed line alone, such as its length, are deleted. An arc split in two keeps its center and gets an Equal relation, so both pieces keep the same radius.

A spline keeps its fit points on the part that remains and gets a new fit point at each cut. Tangent relations at its kept ends stay. A closed spline is trimmed only between two intersections, and opens.

Extending

  1. Click Extend Entities (from the arrow on the Trim Entities button).
  2. Select a line or arc near the end to extend. Before you click, the extension is previewed in orange. Or drag across several entities: each is extended at the end nearer to where the gray line crosses it.
  3. Press Esc to return to Select.

The end goes to the first entity it meets along the line, or around the arc. Construction geometry is not extended to. The new end is tied to that entity as for Trim. A line's length dimension is deleted.

See Also