How Auto Dimension Scheme Works

After you set the Auto Dimension Scheme PropertyManager options and click , the following process occurs.

  1. When you select All features for Scope, the first step performed is feature recognition to deduce the manufacturing features. When recognizing features:
    • All pre-existing features are unchanged. They are not placed in a newly-defined pattern, nor are their faces used to define another feature. For example, if a hole were made a datum, it would not be added to a newly-defined hole pattern, nor would a plane defined as a datum be used to define a slot.
    • The Feature Filters are observed.
    • Features are established giving modeling features priority over features recognized via topology. For example, SOLIDWORKS Hole Wizard, fillet, or chamfer features have first priority.
    • Features are defined giving complex features priority over simple features. For example, the recognition of a counterbore, slot, or pocket takes precedence over a plane or simple hole.
    Feature recognition does not recognize these feature types:
    • Compound hole or compound plane
    • Intersect plane or intersect point
    • Width
    If required, they must be defined as pre-existing features before running Auto Dimension Scheme.
  2. Generating the tolerance schemes for the given set of features, considering Part type and Tolerance type under Settings.
    1. When you select Geometric for Tolerance type, the process begins by applying the tolerances necessary to interrelate the datum features, which can be a combination of orientation, position, and surface profile tolerances.
    2. Size tolerances are applied to all features of size, including all hole types, slots, notches, fillets, chamfers, pre-existing widths, and those included in pattern features.
    3. Dimensions and tolerances are applied to locate each feature and pattern, based on the selected Tolerance type:
      Plus and Minus Applicable plus and minus dimensions are applied to locate every feature, including pre-existing features.
      • The relationships between the reference and tolerance features are not always conducive to standard dimensioning techniques. For example, holes not parallel to the reference features cannot be explicitly located by dimensions. These features typically require dimensions to be directed to the intersection of their axes and another feature, such as a plane (intersect point). You must establish these relationships manually using the Location tool.
      • Surface features are not considered.
      Geometric
      1. Tolerances are applied to interrelate the datum features. For example, if the datum features are three mutually-perpendicular planes, a flatness tolerance is applied to the primary datum feature, a perpendicularity tolerance is applied to the secondary relative to datum A, and a perpendicularity tolerance is applied to the tertiary relative to datums A and B.
      2. Position and circular runout tolerances are applied to locate all features of size, including all hole types, slots, notches, and pre-existing widths.
      3. Surface profile tolerances are applied to locate pockets and surfaces.
      4. Plus and minus dimensions are applied to locate individual plane features, and pre-existing intersection line, plane, and point features.
  3. Creating the display items for the dimensions and tolerances, and placing them in appropriate annotation views, considering the part type, the sketch planes used to define the feature's geometry, and pre-existing annotation views.
    1. A display item is created for each dimension and tolerance.
    2. Tolerance groups are defined. For example, size, datum, and geometric tolerances are grouped together as applicable.
    3. The display items are placed in the appropriate annotation view. The active and pre-existing annotation views are given first priority. If these annotation views are unsuitable, new annotation views are created. The layout of dimensions accounts for the sketch direction. The example below is the same part, but each sketch was extruded along a different axis:
      X-axis
      Y-axis
      Z-axis
    4. Duplicate dimensions are grouped and instance counts applied.
    5. The dimensions and tolerances are laid out, with the objective of giving a clear view of each annotation.