Part Modeling > Sections in Sketch-based Features > To Redefine a Section
To Redefine a Section
A sketch-based feature tool must be closed to redefine a section using this topic. If you want to work within a sketch-based feature tool, see the Note below.
1. With a sketch-based feature tool closed, right-click the section to redefine in the Model Tree. The shortcut menu appears.
2. Perform one of the following actions:
To change only the section dimensions:
1. Choose Edit. The section dimensions show in the graphics window.
2. Double-click the dimension to redefine and type a new dimension in the box, or select a recently used dimension from the list. The section is redefined to the new dimensions.
To redefine the section:
1. Choose Edit Definition. The Sketch dialog box opens. Notice that for dependent sections, the system rolls back to the parent Sketch feature in the Model Tree, enabling you to redefine the parent feature.
2. In the Sketch dialog box, select the sketch plane and the sketch orientation, and click Sketch. The Sketch tab opens and orients the model.
3. Using Sketcher, redefine the section. After you finish, click OK on the Sketch tab. Sketcher closes and the new section is highlighted.
4. Click OK in the Sketch dialog box. The dialog box closes, and the feature geometry shows in the graphics window. The section is also displayed in the Model Tree.
To redefine a dependent section by redefining the parent Sketch feature, refer to the To Create a Sketched Datum Curve topic in the Datum Curves section.
When redefining a dependent section, all changes are applied to the parent Sketch feature and then copied to the dependent section.
You can redefine the section as you work within a sketch-based feature tool. Click Edit from the References tab to use Sketcher. You can also use Edit Internal Sketch from the shortcut menu. Remember that if you are redefining a dependent section, you must click Unlink from the tab to break the association with the parent Sketch feature. Otherwise, Edit will not be available and you must exit the tool to redefine the section.
You can use sketch-based features from previous Pro/ENGINEER releases. However, if an older sketch-based feature cannot be fully referenced, the Section Selection dialog box opens warning you that Use Edge technology will be used to acquire the necessary sketch geometry for the section.
To apply the new dimensions to the feature geometry, regenerate the feature (Model > Regenerate > Regenerate).
You can double-click a section (in the graphics window) to quickly display its dimensions.