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, or ordinate format. You cannot modify the 3D model through driven dimensions.
1. Click > 
Dimension. The Select Reference dialog box opens.
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 a reference type;
entity,
surface, or
any reference.
— Any reference on an entity or surface. Click the arrow next to the icon and select a reference type; entity, surface, or any reference.◦ 
— Tangent point to an arc or circle.
— Tangent point to an arc or circle.◦ 
— Midpoint of an edge or an entity.
— Midpoint of an edge or an entity.◦ 
— Intersection point of two entities.
— Intersection point of two entities.◦ 
— Imaginary line between two points. Additionally, you can specify to draw this imaginary line as horizontal or vertical.
— Imaginary line between two points. Additionally, you can specify to draw this imaginary line as horizontal or vertical.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.
If you select references such that an angular dimension is created, you can specify the type of angle as, inside, outside, or supplementary. Right-click, and select Inside Angle, Outside Angle, Supplementary Angle 1, or Supplementary Angle 2 option.
You can dynamically move the dimension, using the dimension text or leader dragger, and the arrow attachment point hot area. Extension lines are created when you drag the dimension away from its reference. The dimension text flips appropriately as you move the dimension to the opposite side.
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.
) 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.
) 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.