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Offset Entities

Creates copies of a chain of sketch entities at a set distance, tied to the originals by one Offset dimension.

Sketch tab > Offset Entities (on the split button with Mirror Entities and Convert Entities).

The Offset Entities page beside a closed profile of lines and arcs with its offset copy outside it and the Offset dimension shown.

Creating an Offset

  1. Select the lines, arcs, circles or splines to offset. You can also select them after the page opens.
  2. Click Offset Entities.
  3. Set the Distance, and turn on Reverse direction for the other side.
  4. Click OK or press Enter.

The copies follow changes to the originals. The Offset dimension is selected when the page closes; double-click it to change the distance.

Entities to Offset

Entities
The lines, arcs, circles and splines to offset. Each adds its connected chain: the chain grows through every end point where exactly two solid lines, arcs or open splines meet. Construction lines do not join a chain. Select an entity again, or press Del in the box, to remove it.

Circles and closed splines are offset on their own. The lines, arcs and open splines must form one chain without branches.

Parameters

Distance
The offset distance, in the part's units. The default is 5 mm (0.125 in in an inch part); after that, the distance used last.
Reverse direction

Puts the copies on the other side.

Selection Default side
Closed chain, circle, closed spline Outside
Open chain One side, set by the order of the chain

Editing an Offset

Select the Offset dimension in the sketch. Its Dimension section sets the Value, and Reverse Direction moves the copies to the other side.

When an Offset Fails

The status bar gives the reason:

  • The selection branches, or is not one connected chain. Select a single chain.
  • A circle is smaller than an inward distance.

See Also