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Offset

In one sentence: Create an equidistant closed contour around selected sketch geometry, expanding outward for positive values and contracting inward for negative values.

Overview

Workbench: Sketcher · Menu: Sketch → Sketcher tools → Offset
Toolbar: Sketcher Tools · Shortcut: Z, T

Offset generates a new outline that is a fixed distance from the selected edges, following the shape of the original with parallel straight edges and rounded or mitered corners. The result is regular sketch geometry that can be constrained and edited like anything else in the sketch.

Intuition

Think of inflating a balloon around a shape: the balloon follows the outline but sits uniformly further out than the shape's surface. Offset does the same in 2-D: select an outline, set the distance, and a new outline appears running parallel to the original at every point.

Negative offset deflates (shrinks inward). The corner join style controls what happens at sharp corners — whether the offset rounds them (Arc mode) or clips them to a mitered point (Intersection mode).

When to use it

  • Designing a shell or wall of uniform thickness (offset the inner profile to create the outer).
  • Adding an even border around a complex shape (gasket seal, clearance zone).
  • Creating a tool-path offset for machining simulations in the sketch.

When NOT to use it

  • B-Splines and conics — Offset does not support ellipses, hyperbolas, parabolas, or B-Splines as input (these result in an error). Use arcs and lines instead.
  • You need a 3-D offset — use the Part workbench Offset 3D Surface operation, not this Sketcher tool.

Step-by-step walkthrough

  1. Select the edges you want to offset. Use Ctrl-click for multiple edges. (Note: ellipses, parabolas, hyperbolas, and B-Splines are excluded.)

  2. Press Z, T or activate Offset from the toolbar.

  3. The offset handler appears. Drag the mouse to preview the offset distance (positive = outward, negative = inward), or type a value in the task panel.

  4. Choose the join type (see deep dive below) — Arc or Intersection.

  5. Click OK or press Enter. The offset geometry is added to the sketch.

  6. Constrain the offset distance by adding a Distance constraint between a point on the offset and the corresponding original edge.

Parameters

Parameter Type Default Description
Offset distance Distance (mm) Interactive drag Positive = expand outward; negative = shrink inward.
Join type Dropdown Arc How corners are handled: Arc (rounded) or Intersection (mitered). See deep dive below.
Delete original edges Toggle Off If on, the original edges are removed after the offset is created.

Join type in depth

The join type controls what the offset does at sharp corners (where two edges meet at an angle other than 180°).

Arc (default)

At each sharp corner, the offset inserts a circular arc connecting the two offset segments. The arc is centred on the original corner point and has a radius equal to the offset distance.

Use Arc when: - You want smooth, rounded corners on the offset outline (e.g. a blended tool path, a rounded border). - The output will be used as a profile for a Pad or Pocket where sharp corners might cause stress concentrations.

Watch out for: Very small offset distances combined with tight corners can produce tiny arcs that may be difficult to constrain or could cause solver problems.

Intersection

At each sharp corner, the offset segments are extended until they intersect, forming a sharp mitered corner. No arc is inserted.

Use Intersection when: - You need exact sharp corners on the offset (e.g. mitered frames, sheet-metal flanges with crisp corners). - You plan to Fillet or Chamfer the corners separately after offsetting.

Watch out for: At very obtuse angles, the intersection point can be far from the original corner, creating a long spike on the offset. This is geometrically correct but may be undesirable for the design.

Advanced usage

Combining with Trim

After an offset, use Trim to remove any unwanted segments where the offset crosses itself (possible for concave shapes with large offset distances).

Inward offset for pockets

A negative offset distance creates an inward contour — useful for modelling a pocket that has a specific wall thickness. Draw the outer profile, offset by −wall_thickness, and use the inner contour as the pocket profile.

Common mistakes and pitfalls

Offset fails with 'Selection has no valid geometries'

Cause: The selection contains B-Splines, ellipses, or other unsupported conic types.
Fix: Select only lines and circular arcs. Convert or approximate conic curves to arc/line segments before offsetting.

Offset self-intersects for small inward distances

Cause: A concave feature in the original profile causes the inward offset to cross itself.
Fix: Reduce the offset distance, or Trim the crossing segments after the offset is created.

Python API

# Offset is invoked via the GUI handler; no direct Python API is exposed
# for the interactive offset operation in FreeCAD 1.1.
# TODO: verify whether SketchObject.offset() exists as a method.
print("Use the Offset tool interactively; the result is standard geometry.")

See also