Dimension-to-instance association refers to the link between a drawing instance and its related dimension(s). When you dimension a drawing instance, a link is established between the instance and that dimension. Once a drawing instance has been dimensioned, and the part modified after toggling to Model, both the drawing instance and the dimension(s) will update when you re-enter Layout mode. The automatic update is implemented by generating the dimension using the same entities you did when you initially created it. The dimension will appear to scale, but is only updating relative to the geometry it is attached to.

• If/when dimensions are added to a drawing instance and the instance is then moved, scaled, or rotated within its current layout, the dimension(s) will move, scale, or rotate accordingly.

• Several different types of dimensions can be created. The method for creating the different dimensions always falls into one of two categories:

• Entity selection link - When creating this type of dimension, you will be prompted to select an entity from which the dimension will be based.

• Position Menu link - When creating this type of dimension, you use the options available in the Universal Position Menu.

• Depending upon what type of dimension you create, you will be prompted to select an entity, or to choose an option for placement from the Universal Position Menu. For instance, if you attempt to create a linear dimension, you will use the options available from the Universal Position Menu. When creating radial dimensions, you will be prompted to select an arc or circle entity to dimension.

• When the Position Menu is used to create linear, angular, and ordinate dimensions, keep in mind that the options you select to create these dimensions can determine the link that will be established between the instance and its associated dimension(s). This is also true for the changes that you make to the original part file in Model mode.

• Dimensions cannot be tagged or untagged from an instance

• Changing the tagged state of an entity that has a dimension attached to it will cause that dimension to become unattached.

• Various dimensions will have different links.

• If you dimension between a point and the end of an entity in Layout mode, return to Model mode, and delete the point entity, the dimension will be removed from the layout if the "Prevent Non-Associative Dimensions" setting under Tools>Options> Dimensions is enabled. If you have enabled the "Allow Non-Associative Dimensions" setting in the same dialog, and have also enabled the "Correct Displayed Value of Re-associated Orphans" setting, the dimension will be updated. For complete descriptions of these settings, please refer to Tools and Detail.

• If Cursor, Key In, or another combination is used with any other Position Menu option to create a dimension, the program will assume that the instance and dimension are disassociated. As a result, the dimension is never updated if you return to Model mode, modify the geometry, and then return to Layout mode. If Smart Cursor is used to place a dimension, the program assumes the instance and dimension are associated.

• When dimensioning between instances, the instances must be in the same view.

• When dimensioning between layout and instance entities, the layout entities used must be tagged to the instance.

 

Dimension Association Links:

Dimension	Association Type
Linear	Position Menu
Radial	Entity Selection
Angular	Entity Selection and Position Menu
Diameter	Entity Selection
Ordinate	Position Menu
Chamfer	Entity Selection

 

The associations, or links, that are established when each of the available options in the Universal Position Menu is used to place dimensions in Layout mode:

Option	Association	Result
Cursor	No	Dimensions appear, but never update (unless Position Snap is used).
Point	Yes	The dimension is associated to the point entity you select. If you reposition the point and return to Layout mode, the dimension is recalculated according to the point's new position and updated.
EndEnt	Yes	The dimension is associated to the end of the entity you select. If you change the entity and return to Layout mode, the end point is recalculated and the dimension updated.
Center	Yes	The dimension is associated to the center of the entity you select. If you change the center point and return to Layout mode, the center point is recalculated and the dimension updated.
Intrsc	Yes	The dimension is associated to the intersection of two entities. If you change the intersection point and return to Layout mode, the intersection point is recalculated and the dimension updated.
AlongE	Yes	The dimension is associated to a point on a curve at a keyed-in distance. If you change the curve's position and return to Layout mode, the position is recalculated and the dimension updated.
Polar	Yes	The dimension is associated based on the next option you choose from the Position Menu.
Delta	Yes	The dimension is associated based on the next option you choose from the Position Menu.
Key In	No	Dimensions appear, but never update.