Many standard parts are not normally sectioned, but kept intact within a section view. Examples of these basic parts are nuts, bolts, screws, washers, studs, pins, rivets, shafts, keys, cotters, and spokes. In Creo Elements/Direct Annotation, you can secure specific parts or workplanes so that they remain whole in a section view.
Secured parts or workplanes are displayed in their full representation (that is, as an outside view in the direction of the section) within section views. An exception to this occurs when the secured part lies before the section plane. In this case the part is not displayed in the section view.
You can secure multiple parts or workplanes from sectioning in one operation simply by making a multiple selection.
To secure parts from sectioning,
1. Click Annotation and then, in the Setup group, click More.
2. Click Secure. The Secure Parts / Workplanes dialog box opens.
3. Specify the part or the workplane to secure in one of the following ways:
◦ Type the name of the part or the workplane in the Part / WP box.
◦ In the 3D VP, click the part or use the Select tool.
◦ Select the part or workplane from the Structure Browser.
4. Under Influence in general, click the Mode checkbox and select Secure from the drop-down list.
5. Click to complete the operation.
6. To re-allow sectioning of the part or the workplane, repeat the above steps but select Section from the drop-down list in Step 4.
You can also secure a part or workplane in specified views only. In all other views, the part or the workplane is sectioned as normal.
To secure parts or workplanes in specified views,
1. Click Annotation and then, in the Setup group, click More.
2. Click Secure. The Secure Parts / Workplanes dialog box opens.
3. Select the part or the workplane as explained in the preceding procedure and click View in the Influence per view section of the Secure Parts / Workplanes dialog box.
4. Specify the view(s) in one of the following ways:
◦ Enter in the View box.
◦ Click in the Creo Elements/Direct Annotation Viewport.
◦ Select from the Drawing Browser.
5. Under Influence per view, click the Mode check box and select Secure from the drop-down list.
6. Click to complete the operation.
7. To free the view for sectioning, repeat the above but select Section from the drop-down list in Step 3.
You can also specify a part or a workplane to be secure except in certain views. The part or the workplane can only be sectioned in the specified views. To do this, make the appropriate selections in the Influence in general and Influence per view sections.
The possible combinations of securing parts and parts in views are as follows:
Mode
Does this
Part or Workplane Secure, View Secure
Secures the part or workplane from sectioning in all views.
Part or workplane Secure, View Section
Secures the part or workplane from sectioning except in the specified view.
Part or workplane Section, View Secure
The part or workplane may be sectioned except in the specified view, where it is secure.
Part or workplane Section, View Section
The part or workplane may be sectioned in all views.
Note the following concerning secured parts or workplanes:
• When you secure a part or a workplane, an attribute is stored with the 3D model. Therefore you must have write permission for that object to be able to secure it. To secure a part or a workplane in a single view only, you need only have write permission for the owning assembly.
• If you secure a part or a workplane that is already included in an existing section view, you have to update the view to see any changes.
• Shared parts or workplanes are all secured when one of the parts or the workplanes is globally secured.
• Secured parts or workplanes are never visible when the section view mode is set to Secured.
Secure. The Secure Parts / Workplanes dialog box opens.
to complete the operation.