To Modify View Display
If you select multiple views, only the View Display category is displayed in the Drawing View dialog box. All display options are available in this page of the dialog box. Any changes you make are applied to all the selected views.
1. Open a drawing.
2. Right-click the selected view and click Properties. The Drawing View dialog box opens.
3. Click the View Display category. The view display options are displayed in the dialog box. You can modify the view display in the following ways:
◦ Click Use parent view style to set the display of the detailed view to be similar to the parent view display. When cleared, the detailed view display is independent of its parent view and you can modify the display as necessary.
◦ Define how to show the model geometry by selecting a display style from the Display style box:
▪ Default—When you import drawings from Pro/ENGINEER Wildfire 2.0 or earlier releases that were saved with the Default option, this option is retained for these drawings. Once you update these drawings in Pro/ENGINEER Wildfire 3.0, the Default option changes to Follow Environment and the drawings are considered as Pro/ENGINEER Wildfire 3.0 drawings.
▪ Follow Environment—Uses the setting from View > Display Style or the view display style icon in the graphics window.
▪ 
Wireframe—Shows all edges in wireframe style.
▪ 
Hidden Line—Shows all edges in hidden line style.
▪ 
No Hidden—Removes all hidden edge from view display.
▪ 
Shading—Displays shaded views.
| • If you have set the view display mode to Wireframe, Creo Parametric does not erase or redisplay its edges until you change the view display mode to Hidden or No Hidden. • Drawing views saved with the Default option and imported from Pro/ENGINEER Wildfire 2.0 or earlier releases are retrieved in wireframe mode. These views are retrieved in wireframe even after they are saved in Pro/ENGINEER Wildfire 3.0, unless you specifically change the display to follow the environment or change it to shading. To update these views, change the display setting to any other display type and back to any of the Pro/ENGINEER Wildfire 3.0 settings and save the drawing. Once you update these drawings in Pro/ENGINEER Wildfire 3.0, the drawings are considered as Pro/ENGINEER Wildfire 3.0 drawings and the Default option in the Display Style list is no longer available for these drawings. |
◦ Define how to show the tangent edges on the model by selecting a tangent edge display style from the Tangent edges display style box:
▪ Default—Uses the default settings.
▪ 
None—Turns off the display of tangent edges.
▪ 
Solid—Displays tangent edges.
▪ 
Dimmed—Displays tangent edges in dimmed color.
▪ 
Centerline—Displays tangent edges in centerline font.
▪ 
Phantom—Displays tangent edges in phantom font.
◦ Determine whether hidden lines are to be removed for quilts by selecting the appropriate option under Hidden line removal for quilts:
▪ Yes—Hidden lines are removed from the view.
▪ No—Hidden lines are shown in the view.
◦ Define whether to show the skeleton model by selecting one of the following options under Skeleton model display:
▪ Hide—Skeleton model is not displayed.
▪ Show—Skeleton model is shown in the view.
◦ Define whether to enable or disable hidden lines for crosshatches by selecting the appropriate option under Hidden line removal for xhatches:
▪ Yes—Hidden lines are removed from the view.
▪ No—Hidden lines are displayed in the view.
◦ Define how to display cable geometry in the drawing by selecting the required option under Cable display:
▪ Default—Uses the display setting from Tools > Environment.
▪ Centerline—Display cable geometry in centerline font.
▪ Thick—Display cable geometry in thick font.
◦ Define where the drawing should look for color designations by selecting one of the following options under Colors come from:
▪ The drawing—Drawing colors are determined by drawing settings.
▪ The model—Drawing colors are determined by model settings.
|  Model colors and assigned drawing colors in a drawing for a process assembly are always superseded by any existing process assembly colors. |
◦ Define whether weldment cross-sections should be shown in the drawing by selecting one of the following options under Weldment xsection display:
▪ Hide—Weldment cross-sections are not displayed in the view.
▪ Show—Weldment cross-sections are shown in the view.
4. To continue defining other attributes of the drawing view, click Apply and select the appropriate category. If you have completely defined the drawing view, click OK.
| Once you have set the display mode for a specific view, it remains set regardless of the setting in the Environment dialog box, unless you select Default in the Display Style list in the Drawing View dialog box. |