Detailed Drawings > Annotating the Drawing > Dimensioning the Model > Inserting Dimensions > To Insert Additional Dimensions
  
To Insert Additional Dimensions
You can use added or driven dimensions to repeat dimensions that you have already shown. You can add standard type dimensions in the linear, angular, common reference, or ordinate format. You cannot modify the 3D model through driven dimensions.
1. Click Annotate > Dimension. The Select Reference dialog box opens.
2. Select one of the following reference options on the Select Reference dialog box:
◦ — Any reference on an entity or surface.
Click the arrow next to the icon and select one of the following reference types:
▪ — Entity.
▪ — Surface.
▪ — Any reference.
◦ — Tangent point to an arc or circle.
◦ — Midpoint of an edge or an entity.
◦ — Intersection point of two entities.
◦ — Imaginary line.
Click the arrow next to the icon and select one of the following options to create an imaginary line through the specific points:
▪ — Line between two points.
▪ — Horizontal line.
▪ — Vertical line.
This imaginary line is used to calculate the dimension between the selected points.
3. Select the entity or entities that you want to dimension.
You can change the selected reference in the following ways:
◦ Hold down the CTRL key and click the currently selected reference entity to remove the reference.
◦ Hold down the CTRL key and click any other entity to add additional references.
A ghost image of the dimension appears after you select the required number of references. You can drag the ghost image and specify a location to place the newly created dimension.
When you drag the ghost image, the cursor symbolizes the availability of orientation options that you can use to specify to orient the dimension. Right-click to access the orientation options, if available. Based on the proximity of the dimension text to the selected references, the orientation of the ghost image appears slanted, horizontal, or vertical. Additionally, in some instances, you can orient the dimension parallel or perpendicular to an additional reference that you select.
4. Middle-click on the drawing to specify the location for the dimension.
The Dimension ribbon tab becomes active. You can select the available options on the Dimension ribbon to modify properties of the newly created dimensions.
You are still in the dimensioning mode and you can create another dimension. Only the latest created dimension appears selected, and you can use the options on the Dimension ribbon to modify properties of this selected dimension.
During dimension creation, you can select existing dimensions to modify their properties using the ribbon tab. To select multiple dimensions during dimension creation, press Ctrl to select dimensions. For selected multiple dimensions, only common fields are available in ribbon tab, other field appear empty or disabled as appropriate.
5. Middle-click or click in the graphics area to complete the dimension creation.
Dimensioning a Circle or an Arc
If you select the on-entity or surface reference option () on the Select Reference dialog box and select an arc or circle, or both, as a reference, the center point of the arc or circle is considered as the reference to create the dimension. However, if you select the tangent reference option () on the Select Reference dialog box, and select an arc or circle, or both, as a reference, the tangent point of the arc or circle is considered as the reference to create the dimension.
If you select the on-entity or surface reference option () on the Select Reference dialog box and select an endpoint of an arc and a linear geometry as reference, a linear dimension is created. However, if you select the tangent reference option (), and select an endpoint of an arc and a linear geometry as reference, an angular dimension is created between the endpoint of the arc and the linear geometry. Additionally, if you select the on-entity or surface reference option () and select two circular surfaces, a linear dimension is created between their axes.
If you select a circle as a reference to create a dimension, you can right-click and specify diameter or radius as the type of the dimension. Similarly, if you select an arc as a reference, you can specify diameter, radius, angular, or arc length as the type of the dimension. However, if you select multiple entities as reference, and right-click, only the dimension orientation options appear.