Autodimension Tab of the Dimension PropertyManager in Drawings

Specify the following properties to insert reference dimensions into drawing views as baseline, chain, and ordinate dimensions.

To open the Autodimension tab:

  1. In a drawing document, click Smart Dimension Tool_Smart_Dimensions_Relations.gif on the Dimensions/Relations toolbar.
  2. Select the Autodimension tab.

Entities to Dimension

All entities in view Dimensions all entities in the drawing view.
Selected entities Dimensions only the selected entities. Click entities in the drawing view for Selected Entities to Dimension.

Horizontal Dimensions

Scheme Sets the Horizontal Dimensioning Scheme and the entity used as the vertical point of origination (Datum - Vertical Model Edge, Model Vertex, Vertical Line or Point) for the dimensions.
The Horizontal Dimensioning Scheme controls the type of dimension that include:
  • Baseline
  • Chain
  • Ordinate
See Example: Dimension Scheme Types.

By default, the vertical point of origination for the horizontal dimensions is based on the first vertical entity relative to the geometric coordinates x0,y0. You can select other vertical model edges or points in the drawing view.
Dimension placement

Above view

Places dimensions above the drawing view.

Below view

Places dimensions below the drawing view.

Vertical Dimensions

Scheme Sets the Vertical Dimensioning Scheme and the entity used as the horizontal point of origination (Datum - Horizontal Model Edge, Model Vertex, Horizontal Line or Point) for the dimensions.
The Vertical Dimensioning Scheme controls the types of dimension that include:
  • Baseline
  • Chain
  • Ordinate
See Example: Dimension Scheme Types.

By default, the horizontal point of origination for the vertical dimensions (Datum - Horizontal Model Edge, Model Vertex, Horizontal Line or Point) is based on the first horizontal entity relative to the geometric coordinates x0,y0. You can select other horizontal model edges or points in the drawing view.
Dimension placement

Left of view

Places dimensions to the left of the drawing view.

Right of view

Places dimensions to the right of the drawing view.

Origin

Sets the origin for the dimensions. Use an origin instead of horizontal and vertical datums. Select a horizontal edge to set as the zero starting point for all dimensions. To change the origin, select a different edge and click Apply.