Before You Begin

  This section provides the information you need when performing dimensions generation:
First of all, make sure you customize the dimension generation settings settings through Tools > Options > Mechanical Design > Drafting > Generation tab.

 

How are Generated Dimensions Positioned?

Generated dimensions are positioned according to the views that are most representative. In other words, a dimension will appear on a view so that this dimension needs not be also created on another view. Generated dimensions will be positioned according to the following criteria:

  • on the view on which the dimension may be generated.
  • on the view on which the dimension is better visualized. For example, a view on which elements are visualized in non-hidden lines instead of hidden lines.
  • on the view with a bigger scale.
  • on views including more dimensions.
     
    Generated dimensions are not computed in unfolded views.
The dimensions are generated on the views on the condition the appropriate settings were previously activated in Tools > Options > Mechanical Design > Drafting > Generation tab.
 

What About the Dimensions that may be Generated from Constrained 3D Elements?

To make sure the dimensions you need to handle in your session are those expected, here is a list presenting the constrained 3D elements and the resulting associated dimensions after generation.

But first of all, remember that dimensions are generated according to the 3D constraints which belong to the object referenced by the view. In other words, in a view referencing a body, dimensions will be generated only for the constraints which are associated to this body.

A generated dimension is linked to a 3D feature or constraint, and its type cannot be modified into the drawing. For example, a generated diameter dimension cannot be swapped to a radius dimension. 

Note also that for views that are generated from surfaces, only sketched constraints are generated.

Constrained 3D Elements Generated Dimension Types
Sketcher All dimensions: angle, distance, radius, diameter
3D part   Angle, distance
Features: The dimensions below:
  User-defined   All published dimensions of elements included in the user-defined feature
  Pad   Distance
  Pocket   Distance
  Shaft/Groove   Angle

Hole: Constraints and associated dimensions:
  - Simple

 

  
  - Tapered

  - Counterbored

 

 
  - Countersunk

  - Counterdrilled

  - Threaded  
  Fillet constraint variable   Radius/Radii
  Shell   Distance
  Thickness   Distance
  Stiffener   Distance
Assembly constraints   All assembly dimensions

 
 
About threaded hole dimensions

From R18, for thread creation dimensions, NO-DESC_IN_DRAFTING AND DESC_IN_DRAFTING keys defined in 3D standards are not taken into account when creating or updating R18 dimensions. 
For more information on thread creation, refer to chapter

There is no change of behavior when updating pre-R18 thread dimensions. 

A fractional dimension is generated for threads/taps defined in a 3D part which use standards with fraction as a symbolic representation (e.g. G1/8). This dimension is a fake dimension. It will be displayed using the color configured for fake dimensions in Tools > Options > Mechanical Design > Drafting > Dimension tab, Analysis Display Mode category.

Note that although it is a fake dimension, it is always updated properly.

When using ISO standard values, the dimension displayed is a real one (displayed as Mxx) and is based on a key.

When using personal standards including a thread description field, a fake dimension is displayed.
If the description field does not contain any value, a real dimension is used, based on the key and the value of the nominal diameter.

For more information about Threaded Holes and standards, refer to the Creating Threaded Holes section in the Part Design User's Guide.