Use the View Properties dialog box to change attributes for a selected view. Settings on this menu apply only to new or selected views. This includes update settings. These settings generally override global settings.
To modify view properties,
1. Click Annotation and then, in the Setup group, click the arrow next to Properties.
2. Click View.
3. Click the view to modify or select it from the structure browser. Use the Select tool to modify multiple views. The View Properties dialog box opens.
You can also right-click on a view in the viewport or the structure browser for menu access.
4. At top of the menu,
◦ View: Enter a different view to switch to a different view's properties.
5. The General tab includes the following settings:
◦ Name: Change the name of the view. Use the drop-down menu to adjust the view label's style.
◦ Contents: Click to display a table of detailed information about the contents of the view.
◦ Type: Displays the kind of view, for example, Front View or Isometric View.
◦ State: Displays whether the view is up-to-date, the last update date and time, and the Creo Elements/Direct Modeling version of the update.
◦ Scale: Select a scale factor from the list.
◦ Angle: Select a rotation angle for the view from the list.
◦ Configuration: If you have created a configuration in Creo Elements/Direct Modeling, you can select one to assign to the view.
◦ Drawlist: Select an option to determine if and when an assigned configuration's drawlist should be used for the view contents.
6. The Calc Mode tab includes the following settings:
◦ Calc Mode:
▪ Classic:Create a traditional, dimensionable line view with no shading.
▪ Classic + Shaded: Create a dimensionable shaded view.
▪ Graphics: Create a traditional, dimensionable line view with no shading. This mode works well with large models.
▪ Graphics + Shaded: Create a shaded, dimensionable line view. This mode works well with large models.
▪ Shaded: Create a non-dimensionable shaded view (a picture without geometry).
• Shaded views can include annotations created with the 3D Documentation module.
• You can transfer 3D annotations to views created with the Shaded mode (no dimensionable geometry) by using the 100% Transfer mode. To turn 100% Transfer on,
2. In Annotation, expand Transfer 3D Annotations > Behavior.
3. Double-click Create Reference Geo (100% Transfer) and select On.
With 100 % Transfer, you can transfer all 3D Annotations to the 2D drawing. You will still be able to modify dimensions' properties and positions.
◦ EconoFast: Turn the mode on or off.
◦ 2D Association: Select full or limited. See
Update a view for more information.
◦ Solid Parts: Select if you want to ignore or calculate the solid parts in the update mode.
◦ Face Parts: Select if you want to warn, ignore, or calculate face parts in the update mode.
◦ Wire Parts: Select if you want to warn, ignore, or calculate the wire parts in the update mode.
◦ Workplanes: Select if you want to warn, ignore, or calculate the workplanes in the update mode.
◦ Coord. Systems: Select if you want to warn, ignore, or calculate the coordinate systems in the update mode.
◦ Update preserves: Select whether an Update preserves the geometry position or the view center position. See
Change the view positioning strategy for more information.
◦ Clash Handling: You can check Marked Pressfits and Auto Recognition. See
View update settings for more information on clash handling options.
7. The Visibility tab includes the following settings:
◦ Show: Show or hide all or selected hidden lines and tangent lines. Show or hide thread lines.
◦ Calculate: Click appropriate check boxes to have Creo Elements/Direct Annotation calculate symmetry, center, and hidden lines, to remove duplicate hidden lines, and to generate only the outline.
8. The Appear tab includes the Color, Line Type, Pen Size, and Scale Pen of Normal, Hidden and Tangent lines. Select Part / WP Colors from the Normal line color list to use the part or workplane color.
9. The Filters tab includes the following settings:
◦ Small Parts: Remove specified parts either by percentage of view size, or by an absolute size in current units.
◦ 3D Library Parts: Remove these parts from the view.
◦ Full Circles: Remove small circles from the view either by percentage of view size, or by the diameter of the circles.
10. The Section tab includes the following settings:
◦ Secure Mode
The image for each option shows the impact on this drawing:
On—Secured parts that cross the section plane are NOT sectioned. In the image, the screw is a member of the section view, but is not sectioned:
Off—Secured parts that cross the section plane are sectioned. In the image, the screw is a member of the section view and is sectioned:
On, incl. all secured parts in front of section plane — Secured parts that cross the section plane are NOT sectioned, AND secured parts in front of the section plane are displayed:
◦ Rendering: Render the shaded image with the Creo Elements/Direct Rendering module.
13. At the bottom of the dialog,
◦ Set to Default: The default settings for normal view geometry (as specified in the Drawing/View Default Settings menu) can also be applied when modifying views; just click Set to Default and click OK. Note that the checkbox for the current View Properties tab is checked by default.
◦ Copy from: You can copy the settings of an existing view for use as the selections in the Appearance menu. Click Copy from and then specify the view whose settings you want to apply. The fields in the menu are updated to show the selected view's settings.
◦ Copy to: You can copy the settings of the current view to another view. Click Copy to and then specify the view to which you want to apply the settings.
• In the Copy from and Copy to actions, additional properties Contents and Configuration are available for copy.
• When both the checkboxes Contents and Configuration are checked and Drawlist option of configuration is set to “Always” then copy of contents will be ignored and property of the target view will be as per the configuration.
14. If necessary, click Update View to start the update immediately.
15. Click Close when you are finished. Changes are applied as you change settings.
Properties.
