DimXpert Features

DimXpert for parts supports many manufacturing features.

See Discrete DimXpert Feature Types for additional features that build upon DimXpert features.
Feature Example Topology Corresponding SOLIDWORKS Feature
Boss

The dimensioned diameters represent boss features.

An external cylindrical face having a complete 360 degrees of arc No
Chamfer A planar or conical face or swept line. See DimXpert Chamfer Control Options for maximum width and chamfer width ratios Yes.

Chamfer features defined using Angle distance and Distance distance

Cone An internal or external conical face No
Cylinder

The 30, and 50 degree radii represent cylinder features. 		A partial or full internal or external cylindrical face

External faces with complete 360 degrees of arc may be classified as boss features

No
Feature Example Topology Corresponding SOLIDWORKS Feature
Fillet A cylindrical face or swept arc:
  • Up to 180 degrees of arc
  • Cylindrical faces are tangent to supporting faces, when present
  • Chained (concatenated) faces have tangency and equal radii
Yes.

Constant radius fillet features

Counterbore Hole

A typical counterbore hole (left), and a stepped hole with a blind bottom defined as a counterbore hole (right) 		A hole series including two concentric cylinders separated by a plane perpendicular to their axes, with or without a blind end condition of type plane or conic Yes.

Hole Wizard counterbore.

If you define a counterbore hole using the Head clearance or Near side countersink options, DimXpert cannot recognize it as a counterbore hole.

Countersink Hole

A typical countersink hole (left), and a chamfered hole defined as a countersink hole (right) 		A hole series including a cone followed by a concentric cylinder, with or without a blind end condition of type plane or conic Yes.

Hole Wizard countersink.

If you define a countersink hole using the Head clearance or Far side countersink options, DimXpert cannot recognize it as a countersink hole.

Feature Example Topology Corresponding SOLIDWORKS Feature
Simple Hole

(Left) From left to right, a threaded hole with a drill tip bottom, a through hole, and a hole with a flat bottom.

(Right) A compound hole comprised of two cylindrical surfaces.

A hole series including a cylindrical face having more than 180 degrees of arc, with or without a blind end condition of type plane or conic Yes.

Hole Wizard and Simple Hole features

Holes with near side countersinks are recognized as countersink holes (not linked holes)

Intersect Circle A circle derived at the intersection of a cone and plane. The cone must be perpendicular to the plane, and it cannot be created from an ellipse. The cone and plane can be interrupted by a fillet or chamfer. N/A
Intersect Line

An intersect line (blue) forms at the intersection of the part’s bottom plane and the skewed plane (orange).

Intersect lines are typically used for dimensioning. In this example, you may need to locate the intersection of the two planes to the left-hand side of the part to control its length.

A line derived at the intersection of two planes N/A
Intersect Plane

An intersect plane is derived at the intersection of the larger cylinder and conical face.

Intersect planes are typically used to locate the starting or ending location of a tapered surface.

A plane derived at the intersection of a concentric cylindrical and conical face. N/A
Feature Example Topology Corresponding SOLIDWORKS Feature
Intersect Point

An intersect point, shown as an origin, is derived at the intersection of a plane (blue) and a cylinder (orange).

Intersect points are typically used to locate the referencing hole/cylinder. In this example, you may need to locate the hole's pierce point to the right-hand side of the part (creating a horizontal dimension).

A point derived at the intersection of a plane and the axis of a cylindrical or conical face. N/A
Notch Two parallel planes bounded by a plane perpendicular or a cylinder tangent to the side planes, with or without a planar blind end condition No
Plane

Each planar face (gray) represents a single plane feature. You can combine the blue or orange faces to define a compound plane. 		A planar face N/A
Feature Example Topology Corresponding SOLIDWORKS Feature
Pocket

An example of a through pocket (orange) embedded in a blind pocket (blue) 		An internal extruded type closed profile, with or without a planar blind end condition No
Slot A blind square slot (left) and a through slot with radial ends (right) Two parallel planes bounded by two planes perpendicular or two cylinders tangent to the side planes, with or without a planar blind end condition No
Surface A non-prismatic face No
Feature Example Topology Corresponding SOLIDWORKS Feature
Width The pairs of planes that comprise each dimension represent a width feature Two parallel planes with opposing normal vectors No
Wedge Two nonparallel planes with opposing vectors Yes

Create Width/Wedge Feature in the feature selector
Sphere An internal or external spherical face No