The Check Sketch for Feature tool examines sketches for errors in contour that might prevent a feature from being created. It checks for error that are common to all contour types, and, if you select a feature type, it also checks the contour type required for the feature type. When errors are diagnosed, the problem geometry is highlighted.
This example checks a sketch for use in creating a Base Revolve feature.
To check a sketch:
- In an open sketch, click .
- For Feature Usage, select Base Revolve.
Multiple Disjoint Closed is displayed as the Contour type.
- Click Check.
A diagnostic message is displayed, and the corresponding extraneous line is highlighted.
The sketch cannot be used for a feature because an endpoint is wrongly shared by multiple entities.
- Delete the highlighted line.
- Click Check again.
The same message appears and a different extraneous line is highlighted.
The sketch cannot be used for a feature because an endpoint is wrongly shared by multiple entities.
- Delete the highlighted line.
- Click Check again.
A new message indicates that the highlighted line is not connected to the intersecting lines.
The sketch has more than one open contour.
- Trim one end of the line and extend the other end.
- Click Check again.
Now all the errors have been found and corrected.
No problems found. The sketch contains 1 closed contour(s) and 0 open contour(s).
- Click Close.
To create the base revolve feature:
- Click Revolved Base/Boss
(Features toolbar) or .
- Select the line shown as the axis of revolution.
- Click
to complete the feature.
