When you select the View Wizard command to define a part view, you can use the View Wizard command bar to make changes to the drawing view before it is placed on the sheet.
You can select the border of an existing drawing view to modify it using the Drawing View Selection command bar and the Drawing View Properties dialog box.
Drawing View Style Mapping
Specifies that the drawing view will use a predefined style, which is set on the Drawing View Style tab of the Solid Edge Options dialog box.
When the Drawing View Style Mapping button is cleared, you can select and apply individual styles. Choose the style from the Drawing View Style list.
Drawing View Style
Selects a style for the drawing view. This option is not available when Drawing View Style Mapping is enabled.
Caption
Displays the primary caption text defined in the drawing view style for the selected drawing view. Caption text may consist of plain text, property text, and symbols.
You can add and edit multiple lines of primary caption text by typing in the box. You also can modify the content using the Caption tab (Drawing View Properties dialog box).
Show Caption
The top portion of the Select Caption list selects the caption types (primary, secondary) to be displayed for the currently selected drawing view or view annotation.
The bottom portion of the Select Caption list specifies whether to display the values for property text codes (%AS, %VS, %VR, and %LN).
Show Primary Caption
Specifies that the content defined for the Primary caption is displayed.
You can modify the caption content for the selected drawing view using the Caption tab (Drawing View Properties dialog box).
Show Secondary Caption
Specifies that the content defined for the Secondary caption is displayed. The secondary caption text always appears below the primary caption text.
You can create and modify the secondary caption content for the selected drawing view using the Caption tab (Drawing View Properties dialog box).
Note:
Even when the Show Primary Caption or Show Secondary Caption option is checked, when any of the following property text codes are part of the caption, you must also select the matching property from the Show Caption list to show its value in the caption.
Show Suffix
When a section view, detail view, or auxiliary view is selected, and when %AS is defined in the caption, displays the caption suffix.
Show Annotation Sheet Number
When a section view, detail view, or auxiliary view is selected, and when %LN is defined in the caption, displays the sheet number where the view annotation--the cutting plane, viewing plane, or detail envelope--is located.
Show View Scale
Displays the view scale in the caption when %VS is defined in the caption text.
Show Angle of Rotation
Displays the view rotation angle in the caption when %VR is added to the caption text.
Note:
Primary captions, secondary captions, and view annotation captions can be defined globally in the Drawing View style. To learn how, see these Help topics.
You also can add a primary caption to a selected drawing view using the Caption box on the Drawing View Selection command bar.
Saved Settings 
Opens the Saved Settings dialog box for you to name, save, and delete saved settings for drawing views. You also can select an existing saved setting using the list button. Only saved settings that apply to the current model type are listed.
If you select blank from the saved setting list, the drawing view formatting is specified by the current set of options on the command bar.
Drawing View Wizard Options
Opens the Drawing View Creation Wizard (Drawing View Options) for you to specify content and display options based on whether the drawing view is an assembly, part, or a sheet metal model.
Drawing View Layout 
Opens the Drawing View Creation Wizard (Drawing View Layout) for you to select additional views to place along with the primary view. You also can change the orientation of the primary view.
View Orientation 
Changes the model view orientation before the drawing view is placed. You can select a Solid Edge default view or a user-defined named view. The default view options include Front View, Top View, Right View, Iso View, and Trimetric View.
Best Fit
Assigns the calculated best fit scale to all of your new part views. The scale value is shown in a box on the command bar.
Set View Scale
Set the scale of the new view to match the current sheet scale.
Scale List
Selects a standard drawing scale to use to place the selected views, for example, 2:1.
The specified ratio defines the size of the drawing in relation to the size of the real-world object. For a 2:1 ratio, the 2 represents the size of the drawing and the 1 represents the size of the real-world object.
Scale value
Specifies a custom scale value, for example, 10.000.
Note:
Scale values are defined in the Drawing View Scales section of the Custom.xml file, in the Solid Edge Preferences folder. For more information, see the Help topic, Add custom drawing view scales to Solid Edge.
Set Sheet Scale
When selected, sets the sheet scale to match that of the drawing view being placed. If this is the first or primary drawing view placed on the sheet, then this automatically sets the view scale for all drawing views subsequently added. This ensures that the scale of all drawing views on the sheet is consistent.
This button is selected by default if the sheet scale is already linked to another drawing view on the sheet. You can use the Set Sheet Scale shortcut command on the sheet tab to determine which drawing view it is associated with.
When deselected, the new view is placed using the value shown in the Scale List. The sheet scale and the drawing view scale are not associative.
Model Display Settings
Opens selected tabs in the Drawing View Properties dialog box for you to change display settings before you place the drawing view(s):
Display tab (Drawing View Properties dialog box--In an assembly, you can choose to display selected parts in the views. These settings are applied to all the views you create.
Sections tab (Drawing View Properties dialog box)--Selects a 2D section to be applied to the drawing view.
Shading and Color tab (Drawing View Properties dialog box) --Applies model colors and shading to the drawing view.
Shading Options
Specifies color or grayscale, shading, and edge visibility for the drawing view.
Not Shaded
Displays color with visible and hidden edges, but no shading.
Shaded
Displays color and shading, but no edges.
Shaded with Edges
Displays color and shading with visible edges.
Grayscale Shaded
Displays grayscale and shading, but no edges.
Grayscale Shaded with Edges
Displays grayscale with visible edges.
Use Model Colors
Applies model colors to drawing view edges and hatching. A drawing view that uses model color goes out of date when the color is changed in the model.