Hide Table of Contents

Measurement PropertyManager

The first step in creating a TolAnalyst study is to specify the measurement as a linear dimension between two DimXpert features.

Examples

This measurement is the overall length of the three-part assembly.

 

 

This measurement is the gap between a hole and a shaft.

You can define measurements between any of the following DimXpert features. When the selected features are a combination of plane, line, or axis types, they must be parallel to one another. Surface types require that you use an exact point.

  • Point types: Sphere, Intersect Point

  • Axis types: Boss, Cone, Cylinder, Simple Hole, Counterbore Hole, Countersink Hole, Slot

  • Line types: Intersect Line

  • Plane types: Notch, Plane, Width

  • Surface types: Surface

To define a measurement:

  1. Select faces of two features for Measure From and Measure To to establish the measurement.

The selection of which feature is Measure From versus Measure To can affect the results.

A linear dimension appears in the graphics area.

  1. Click to place the dimension.

The Message box turns from yellow to green, indicating the measurement is defined.

  1. Select the PropertyManager options as necessary.

  2. Click .

PropertyManager Options

Measure From and Measure To

Selected face . Select faces of two features to establish the measurement.

Specify Exact Point. Directs the measurement to a specific point on one or both features. This restricts the computation of the worst case results to be at the specified point instead of considering the entire boundary or axis of the feature.

The explicit point can be a vertex point or reference point (defined using Insert, Reference Geometry, Point). An explicit point is coincident with the plane or axis of the feature, but is not required to lie within the feature's boundary or axis endpoints.

These examples illustrate the use of explicit points using reference points.

The measurement is defined using reference points created at the top of the two pins.

 

 

The reference points are placed directly opposite one another on the surfaces of the two planes.

Center, Minimum, and Maximum. Directs the measurement to the center or edge of the feature. These options are available when you select a feature-of-size.

Examples:

 

The minimum and maximum side options are supported for these feature types:

  • Boss

  • Cylinder

  • Notch

  • Simple Hole

  • Slot

  • Width

Measurement Direction

Sets the direction of the dimension when the measurement is applied between two axes (including slot axes).

X, Y, and Z. These options are relative to the coordinate system and are enabled for each axis that is perpendicular to the axes of the features.

N. Normal. Orients the dimension at the shortest distance normal to the two axes.

U. User defined. Orients the dimension along a selected line or normal to a selected planar face.

The example illustrates two measurements defined to evaluate the offset between two bearing bores, where one is defined along the X-axis and the other along the Z-axis.



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:   Measurement PropertyManager
*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 2012 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.