FeatureWorks Options
Allows you to customize FeatureWorks options and set default values.
To specify default options for Feature
Recognition:
-
Click FeatureWorks Options 
(Features toolbar) or Insert,
FeatureWorks, Options.
The Options dialog box appears.
Select from the following options, then click
OK.
General
Overwrite
existing file. Create the new features in the existing part document,
and replace the original imported body.
Create new
file. Create the new features in a new part document.
Prompt
for feature recognition as part opens. When selected, feature recognition
begins automatically when you open a part as an imported solid body in
a SolidWorks part document from another system.
Dimensions/Relations
Enable Auto Dimensioning
of Sketches. Automatically adds dimensions
to recognized features.
Scheme.
Sets the dimensioning scheme as Baseline,
Chain, or Ordinate.
Placement.
Sets the Horizontal and Vertical placement of dimensions.
Relations.
Add constraints
to sketch. Adds
a Fix relation to each entity
in a sketch, fully defining the sketch. If this check box is not selected, the sketch entities remain under
defined. FeatureWorks recognizes concentric relations.
Refer to this reference
topic for details about recognition of relations and constraints.
Resize Tool
Recognition
Order. Sets the order in which the
resize tool recognizes features. For
example, if you placed Cut Revolve
above Hole, the software tries
to first recognize the feature as a cut revolve. If that recognition fails,
then the software tries to recognize the feature as a hole.
Automatically recognize child features when
using Edit Feature. While using Edit
Feature to recognize faces on imported bodies, recognizes child
features of the face. Select Yes,
No, or Prompt.
Advanced Controls
Diagnose
Allow
failed feature creation. Allows the software to create features
that have rebuild errors. If this check box is not
selected, the software fails to recognize any features if one or more
features have a rebuild error.
Perform
body difference check. Compares
the original imported body to the new body after feature recognition.
A body difference occurs only if you
during feature recognition. This check box is available only if you select
Create new file under File.
Performance
Do not perform feature intrusion check.
When you select this check box, the software does not check for features
that intrude upon one another during Automatic Feature Recognition.
Do not perform body check. When you
do not select this check box, the software periodically checks the body
during feature recognition. If this check box is selected, the software
does not check the body for any errors (resulting in faster performance.)
Holes
All other types of Hole Wizard holes are
recognized as Hole Wizard Legacy
type holes.
To recognize Hole Wizard holes, FeatureWorks must be able
to reference the SolidWorks Toolbox’s swbrowser.mdb
file. For example, if you reference a shared toolbox on a network, you
must be connected to that network to be able to recognize Hole Wizard
holes using FeatureWorks.
Automatic Recognition
Combine
Fillets. When selected, automatically combines fillets with the
same radius into a single feature.
Combine
Chamfers. When selected, automatically combines chamfers with the
same angle and width into a single feature.
Combine
Holes. When selected, automatically combines holes with similar
parameters on the same plane into a single feature.