When you select the View Wizard command, the Drawing View Creation Wizard guides you through the process of selecting and placing one or more drawing views.

Drawing View Creation Wizard page	Settings
Select Model dialog box	You select the model from which the drawing views are derived.
Drawing View Options	Sets options for creating the view, based on the Solid Edge model type. For example: When creating a drawing of an assembly, you can choose a display configuration, a PMI model view, or a zone to control the display of the parts in the drawing view. When creating a drawing view of a weldment, you can specify the process-specific view of the weldment you want to place. Note: You can select the Advanced button on the Drawing View Options page to set limits on edge creation using the Advanced Edge Display Options dialog box.
Drawing View Orientation	Specifies the primary view orientation, such as front or right or iso. Note: You also can select the Custom button to define a perspective view of the model using the Custom Orientation dialog box.
Drawing View Layout	Specifies additional views to place along with the primary view.

Before you click to place the drawing view, you can use the View Wizard command bar to choose:

• Drawing view style

• Drawing view caption

• Drawing view scale

• Edge display style

• Shading

On the Drawing View Wizard (Drawing View Orientation) page, if you selected multiple model views to place at once, then the View Wizard command ends when you click the drawing sheet. If you place just one view, then the command remains active. You can:

• Create additional folded views by clicking to the right, left, top, or bottom of the initial or selected view.

• Create pictorial views by clicking diagonally to the top-right, top-left, bottom-right, or bottom-left of the initial or selected view.

• Right-click to end drawing view placement mode.

You can change the appearance of a drawing view after you place it. Select the border of the drawing view you want to modify, and then make display changes using the options on the Drawing View Selection command bar. For more extensive options, select the Properties button on the command bar to open the Drawing View Properties dialog box.

Multiple model or assembly documents can be attached to a draft document. After you place the first part view in a document, you can select the View Wizard command again to place additional part views. The next time you select the command, the Select Attachment dialog box is displayed. This dialog box lists the documents that are currently placed in the draft document, and it allows you to browse for another part or assembly to use as the basis for the next part view.

• Create drawing views of a part or assembly

• Create an alternate position assembly drawing view

• Create a draft quality view

• Drawing view creation

• Documenting multiple parts in one Draft document

• Drawing View Selection command bar

• Create drawing dialog box

• Drawing View Creation Wizard (Drawing View Options)

• Drawing View Creation Wizard (Alternate Position Assembly)

• Drawing View Creation Wizard (Drawing View Orientation)

• Drawing View Creation Wizard (Drawing View Layout)

• View Wizard command bar

• Drawing View Properties dialog box

• Custom Orientation dialog box

• Select Model dialog box

• Select Attachment dialog box