Hide Table of Contents

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

Sphere

An internal or external spherical face

No



Provide feedback on this topic

SOLIDWORKS welcomes your feedback concerning the presentation, accuracy, and thoroughness of the documentation. Use the form below to send your comments and suggestions about this topic directly to our documentation team. The documentation team cannot answer technical support questions. Click here for information about technical support.

* Required

 
*Email:  
Subject:   Feedback on Help Topics
Page:   DimXpert Features
*Comment:  
*   I acknowledge I have read and I hereby accept the privacy policy under which my Personal Data will be used by Dassault Systèmes

Print Topic

Select the scope of content to print:




x

We have detected you are using a browser version older than Internet Explorer 7. For optimized display, we suggest upgrading your browser to Internet Explorer 7 or newer.

 Never show this message again
x

Web Help Content Version: SOLIDWORKS 2011 SP05

To disable Web help from within SOLIDWORKS and use local help instead, click Help > Use SOLIDWORKS Web Help.

To report problems encountered with the Web help interface and search, contact your local support representative. To provide feedback on individual help topics, use the “Feedback on this topic” link on the individual topic page.