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Line / Polyline

In one sentence: Draw a single straight line segment (Line) or a connected chain of line segments where each endpoint automatically becomes the start of the next (Polyline).

Overview

Workbench: Sketcher · Menu: Sketch → Sketcher geometries → Line / Polyline
Toolbar: Sketcher Geometries · Shortcut: G, L (Line) · G, M (Polyline)

Line and Polyline are the most fundamental drawing tools in Sketcher. A Line creates one segment; a Polyline creates a chain of segments, automatically adding a Coincident constraint between consecutive endpoints. Both tools leave the resulting geometry unconstrained until you apply length, angle, and positional constraints.

Intuition

A Line is like drawing a single stroke of a pencil between two points. A Polyline is like keeping your pencil on the paper and making a series of strokes — each new stroke starts exactly where the previous one ended, so the chain is always connected.

The key practical difference: if you draw a closed shape (a rectangle, a triangle) using Polyline, the last click near the first vertex will close the loop automatically. Drawing the same shape with individual Line commands requires you to manually add Coincident constraints at each junction.

When to use it

  • You need any straight-sided shape: profiles, cross-sections, brackets, plates.
  • You want to draw a connected outline quickly without manually applying coincident constraints at every corner (Polyline).
  • You want a single construction axis or reference line (Line in construction mode).

When NOT to use it

  • You need a rectangle — use Create Rectangle instead; it draws a closed, constrained rectangle in one step.
  • You need a regular polygon — use Create Regular Polygon.
  • You want to connect two existing endpoints — you can still use Line, but adding a Coincident constraint to each endpoint after drawing is equivalent and more explicit.

Step-by-step walkthrough

Single line

  1. Press G, L or activate Sketch → Sketcher geometries → Line.
  2. Click the start point in the viewport.
  3. Click the end point. A line segment appears; a length dimension is not yet applied.
  4. Press Esc or right-click to exit line mode, or click a new start point to draw another separate line.
  5. Constrain the line — set its length with Dimension or Distance, and its angle or endpoint positions.

Polyline (chain of connected lines)

  1. Press G, M or activate Sketch → Sketcher geometries → Polyline.
  2. Click the start point.
  3. Click successive waypoints. Each click completes the previous segment and starts the next; a Coincident constraint is applied automatically at each junction.
  4. To close the polyline: click near (or exactly on) the starting point. A closing line with a Coincident constraint appears.
  5. Press Esc or right-click to finish without closing, leaving the last point unconnected.

Tip

While drawing a Polyline, press M to toggle between Line and Arc mode. This lets you mix straight segments and arc segments in a single connected chain without leaving the command.

Parameters

Both tools share the same implicit parameter: the two endpoints set by clicks. After drawing:

Parameter Type Applied via
Length Distance Dimension or Distance
Angle Angle Dimension or Angle
Endpoint position Coordinate Lock Position or Coincident
Horizontal / Vertical Geometric Horizontal/Vertical

Advanced usage

Mixed line-arc polyline

Inside Polyline mode, pressing M toggles between straight-line and arc sub-modes. In arc mode, three clicks define an arc instead of a line. The tangency at the junction is automatically maintained as a Tangent constraint, giving you smooth blended outlines in a single operation.

Construction lines

While drawing (or after selecting a line), press G, W or toggle the Construction mode button in the toolbar to convert the line to a construction (dashed) element. Construction lines participate in constraints but do not form part of the sketch profile passed to Part Design.

Common mistakes and pitfalls

Polyline not closed — last segment floats

Cause: You pressed Esc before clicking back on the first vertex, leaving the last endpoint free.
Fix: Add a Coincident constraint between the last endpoint and the first vertex, or delete the unwanted last segment and redraw ending exactly on the first point.

Line length cannot be set — over-constrained

Cause: Both endpoints are already fully constrained (e.g. each is coincident with another fully constrained vertex), so adding a length constraint would be redundant.
Fix: Remove one of the endpoint constraints and replace it with the length constraint; or accept that the length is derived from the endpoint positions.

Python API

Minimal example

import FreeCAD as App
import Sketcher
import Part

doc = App.activeDocument()
sketch = doc.getObject("Sketch")

# Add a horizontal line from (0,0) to (30,0)
idx = sketch.addGeometry(
    Part.LineSegment(App.Vector(0, 0, 0), App.Vector(30, 0, 0)), False)

# Constrain start to origin
sketch.addConstraint(Sketcher.Constraint("Coincident", idx, 1, -1, 1))
# Fix the length
sketch.addConstraint(Sketcher.Constraint("Distance", idx, 30.0))
# Enforce horizontal
sketch.addConstraint(Sketcher.Constraint("Horizontal", idx))
doc.recompute()

Key properties

Part.LineSegment returned by sketch.Geometry[idx]:

Property Type Description
StartPoint App::Vector Coordinates of the first endpoint (vertex 1).
EndPoint App::Vector Coordinates of the second endpoint (vertex 2).
Length float Current length in mm; read-only (set via constraints).

See also