Some or all hole dimensions from a hole parameters
(except if these parameters cannot be associated with an existing
geometrical element to generate dimensions: diameter of a tapered
hole out of the part, depth for a blind hole setting a through
hole, etc).
Pad/Pocket length: if two limits are defined,
two dimensions will be generated between the sketch plane and
each limiting face, and sketch constraints.
Multi-Pad/Multi-Pocket lengths, and sketch
constraints.
Shaft/Groove distance constraints that are
parallel or perpendicular to the shaft/groove axis direction,
distance between shaft/groove axis and point and/or straight
line and/or circle (arc or complete) as a half dimension diameter
if the shaft/groove is not complete (value of the single angle
or total of the 2 less than 360 degrees, as regular diameter
if the shaft/groove is complete, angle, and sketch constraints.
Chamfer features; dimensions are generated
according to the Part Design chamfer feature definition: for
a chamfer with a length x length definition, the dimension format
will be distance x distance, whereas for a chamfer with a length
x angle definition, the dimension format will be distance x
angle dimension. However, you should be aware of the fact that
if tolerances are applied to chamfer parameters, only the tolerance
applied to the first parameter will be generated. Chamfer dimensions
cannot be edited, but they can be modified via the Dimension
Properties toolbar and the Edit Properties
command.
Thread features; thread diameter, depth and
pitch parameter dimensions can be generated. Dimension generation
automatically generates a thread symbolic representation.
Warning:
Any tolerance attached to the pitch or
diameter parameter will not be generated.
Generating a pitch parameter dimension
requires the generation of the corresponding thread diameter
parameter dimension.
If the thread is not a metric one, the
prefix will be a diameter symbol instead of the letter M.
You could select User Feature
and explore them in order to find Part Design features allowed
in Generative command.
The command will recursively search each compatible internal
Part Design features (in the same way User Feature
containing other User Features) in order to show
parameters (if nothing could be analyzed by generative command,
no parameter will appear).
Moreover, user can immediately select all of them in generative
command list as if User Feature does not exist.
Only published parameters (during User Feature creation)
are seen in list and corresponding dimensions could be created.
Important:
Dimensions are associated with the design of a part, including
the Mean Dimension behavior.
When parameter tolerances are still defined, they are set
to the dimension tolerances.
Modifying dimension tolerances modifies the parameter tolerances
and vice-versa.
A generated dimension is always created in an annotation
plane parallel to the related feature internal parameter plane
and this annotation plane is not necessarily the active annotation
plane:
If an annotation plane parallel to the feature internal
parameter plane already exists, the dimension is created
in this annotation plane,
Otherwise a new annotation plane is created parallel
to the feature internal parameter plane.