Known Limitations of Compare

Known Limitations of Compare Documents

  • When you compare two different document types (such as a part document and an assembly document), only the common properties are compared. The comparison results are classified into File Properties and Document Properties.
  • Compare Documents cannot be used for documents in "view only" mode. However, it can be used for documents in "read only" mode.

Known Limitations of Compare Features

  • Compare Features works on SOLIDWORKS parts that have parameterized features. Parameterized features are those features whose dimensions you can modify. An example of a part without parameterized features is an imported part whose only feature is 'Imported1'. Compare Features also compares appearance properties, including colors, optics, and textures.
  • Compare Features works only on solid features.
  • Compare Features uses the feature names as the main criteria for pairing features.

    If you change the name of identical features in the two parts, Compare Features classifies these features as unique. For example, the feature Hole-1 in Part A is identical to the feature Hole-1-Mod in Part B. The only difference is the name. When compared, both Hole-1 and Hole-1-Mod are classified as unique features instead of modified features.

    If you have two parts with identical features, but from two different language versions of SOLIDWORKS, the features are classified as unique because their names are different.

  • Compare Features does not compare thicken, cavity, shape, deform, combine, join, split, move/copy, or delete body features. These features appear under Uncompared Features in the tree on the Compare Features Results CompareFeatures_ResultsTab.gif tab of the Compare Task Pane.
  • Compare Features cannot meaningfully identify completely dissimilar parts.

    If two completely dissimilar parts have features with the same name and type, Compare Features compares these features and tries to classify them as identical or modified.

  • Compare Features requires that the two parts be in the same position with respect to the origin. If one of the parts has been moved, the results may be incorrect.

Known Limitations of Compare Geometry

  • Compare Geometry treats each solid as a single entity. It does not compare the features of the parts, and cannot point out differences in feature parameters. To compare features, click Utilities > Compare Features.
  • When comparing analytic faces (planes, cylinders, spheres, and so on) the equations of the underlying surfaces are used. However, with spline faces, a discrete sampling technique is used to compare the equality of the underlying spline surfaces. Under certain circumstances, the comparison of spline faces may give inaccurate results.
  • The volume difference computation for parts containing a large number of spline faces may occasionally fail. You can turn the volume comparison option off for parts containing a large number of spline faces.
  • If the faces are sliver faces or have very small areas, the results for unique and modified faces may be incorrect.
  • If FeatureWorks is installed on your machine and you open a part without parameterized features, the following occurs:

    FeatureWorks displays a dialog box that asks if you want to proceed with feature recognition for the imported part. Click No.

    If you click Yes, which starts feature recognition, do not click Run Comparison in the Compare Features Task Pane. Running the two simultaneously can have undesirable results.

  • Compare Geometry requires that the two parts (or assemblies) are in the same position with respect to the origin. If one of the parts (or assemblies) has been moved, the results may be incorrect. Select Align parts to compare geometrically similar bodies located in different positions, relative to the origin.