Create drawings from models (Creo Elements/Direct Annotation) > Modify views > Change the contents of views > Manage parts or workplanes in views
Manage parts or workplanes in views
Use the Manage commands to define the component list of a:
2D view within the Creo Elements/Direct Annotation Module.
Docuplane within the 3D Documentation Module.
If you select a docuplane belonging to a multi-section, Creo Elements/Direct Modeling applies any changes you make to every other docuplane of that multi-section.
The following help information describes the Creo Elements/Direct Annotation scenario.
Removing parts from a view can both simplify the representation, and also speed up drawing generation performance.
The following graphic illustrates the removal of several components from a 2D drawing:
1. Shows the 3D model before creating the 2D drawing. This view is similar to the auxiliary viewport that is displayed when Creo Elements/Direct Annotation asks you to select the components to be removed.
2. Shows the initial 2D drawing containing all components. After selecting this view in Manage, Creo Elements/Direct Annotation displays the auxiliary viewport. Parts p1, p2, and p3 were removed using the Rem Selected filter.
3. Shows the redrawn 2D drawing with the specified components removed.
To remove or add components from a view,
1. Create the initial 2D drawing in the usual manner.
2. Click Annotation and then, in the Setup group, click Manage. The Manage Parts / Workplanes dialog box opens.
3. Specify one or more views and wait for Creo Elements/Direct Annotation to display the auxiliary viewport. (When multiple views are selected, only a subset of the options is available.)
4. Click Removed or Remaining to choose which parts to display in the auxiliary viewport.
5. Select one or more of the following size filter options if necessary:
Threshold %
The relative size of each part or workplane is calculated for both directions (width and height). By default, this size is relative to the total view size, but the size reference can be changed with the options Parent and Siblings described below.
Only parts or workplanes where the relative size is below the threshold for width and height are considered for adding or removing.
To eliminate the sleeve in the following, a threshold of 50% was set:
The size reference for a part or workplane is not the view's size, but the size of the parent assembly.
The reference size (view size or parent assembly size) is divided corresponding to the number of parts inside the parent assembly.
Rem Small or Add Small
Finally, after defining the rules, you can apply them to remove or add parts by size criteria.
6. Under Other Filters, if necessary, click Rem Selected or one of the following options to remove parts from or add parts to the 2D drawing:
Rem Lib Part or Add Lib Part
Allows specification of library parts, such as screws and bolts.
Rem Invisible or Add Invisible (Only in Creo Elements/Direct Annotation)
Specify whether or not to remove or parts or workplane from the view's component list that are not visible . (Creo Elements/Direct Annotation first scans the 2D geometry in the view to identify which parts or workplanes are actually visible in this view.)
This option is particularly powerful for detail views or for assemblies with many hidden parts asit can reduce the time needed to update views significantly.
You must update the view at least once before using this option.
Rem All or Add All
Use Rem All to remove all parts under the view owner from the view's component list. Use Add All adds all available parts or workplanes to the view component list.
Rem Container or Add Container
Add Container and Rem Container add or remove containers created in the Part & Assy menu.
Rem Selected or Add Selected
Use Rem Selected and Add Selected to control manually which parts or workplanes should be included in the view component list. When a single view is selected, Creo Elements/Direct Annotation displays the parts or workplanes removed (or remaining, see Step 5), in the auxiliary viewport. When multiple views are selected, Creo Elements/Direct Annotation shows all parts or workplanes in the preview.
Create Part Group
Use the Removed and Remaining options to create part groups representing the removed or remaining parts of the view. The part groups are added to the viewset owner and can be used to show all removed parts, to save only remaining parts, or to modify the components list of other views in the same way.
This option is valid for single view selection only.
Click a view in the Creo Elements/Direct Annotation viewport to add or remove components by copying another view's component list. You must clear the selected view's component list where you want to add or remove components, before you copy another view's component list to the selected view.
Workplanes are not included in a parts group.
7. Click to end your selection.
8. Update the view.
Creo Elements/Direct Annotation does not handle coordinate systems exactly the same way as it handles parts. A coordinate system is displayed in the auxiliary viewport even when it is not in the components list. If a coordinate system is removed from the components list without removing its related part, it is not displayed in the auxiliary viewport. To add such a coordinate system to the view component list, you must double-click the coordinate system in the Creo Elements/Direct Modeling Structure Browser.