Drawing View dialog box

Edits properties of drawing views. Specifies a model and setup for a base view.

Note: If the Enable Background Updates application option is selected, raster views are displayed until calculation of precise views is complete. For more information, see Work with raster views.

Tip: Default settings and values in the Drawing View dialog box are defined in the current standard and can be changed by using Style and Standard Editor.

Access:

To create a view, click the Base command on the Place Views tab. To edit a view, right-click the view in the browser or the graphics window, and then select Edit View from the menu.

Component tab

Selects the source file and the representations to use in a drawing view.

File	Specifies the source part file to use for the drawing view. Click the arrow to select from the list of open files or click the drop-down arrow next to File. Select Open an existing file to browse for a non-vaulted file. Select Open from Vault to browse for a file in the vault.
Representation:
View	Lists names of assembly design view representations. Select a view representation from the list. This option is available when the selected file is an assembly that contains defined design view representations. Select the Associative check box to update the drawing when changes are made to the associative design view representation in the assembly environment.
Position	Selects a positional representation to show in the view. This option is available for base view creation.
Level of Detail	Selects a level of detail representation to show in the view.
Sheet Metal View	Available only when the selected model is a sheet metal file. Folded Model creates a view of the sheet metal folded model. Punch and bend annotations are not available for folded model views. Flat Pattern creates a view of the sheet metal flat pattern. Available only if a flat pattern exists in the sheet metal file. Recover Punch Center controls if punch centers are included in the view. Punch centers must be recovered to create punch notes or punch tables. Available only if Flat Pattern is selected.
Presentation View	Available only when the selected file is a presentation document. Specifies the presentation view to use. To associate the drawing view with the presentation, select the Associative check box above the view list.

Model State tab

Specifies weldment state and iAssembly or iPart member to use in a drawing view. Specifies reference data such as line style and hidden line calculation method.

Weldment	Available only when the selected file contains weldments. Click the weldment state to represent in the view. All components in preparation state are listed below the Preparation separator line.
Member	For an iAssembly factory, selects the member to represent in the view.
iPart Member	Selects the sheet metal iPart member to represent in the view. Available only if a sheet metal iPart is selected as the source file.
Reference Data	Line Style sets the line style for the reference data. Click the arrow to select the style of Referenced Parts, Parts, or Off. Hidden Line Calculation specifies if hidden lines are calculated for All Bodies or Reference Data Separately. Margin sets the amount of area outside the normal view boundary that the view boundary extends. Controls the amount of reference geometry shown in the view. Note: Parts with the BOM Structure set as Reference are not included in the formula for creating the default size of the view bounding box. As a result, the Reference parts can be clipped in drawing views. To extend the size of the view bounding box, increase the Margin value on the Model State tab of the Drawing View dialog box.

Display Options tab

Sets the display options for the drawing view. Select an option to add it to the view. Clear the check box to remove it from the view. Only those options applicable to the specified model and the view type are available.

All Model Dimensions	Associates model dimensions to the view. Select the check box to retrieve the model dimensions. Only those dimensions that are planar to this view and were not used in existing views on the sheet display. Clear the check box to place the view without model dimensions. If dimension tolerances are defined in the model, they are included in the model dimensions.
Model Welding Symbols	Associates model welding symbols to the view. Select the check box to get the model welding symbols. Clear the check box to place the view without model welding symbols.
Bend Extents	Sets the visibility of sheet metal bend extents in the view. Select the check box to display the bend extents. Clear the check box to hide them. Note: The display of bend extents is determined by the Sheet Metal Bend Extend object default.
Thread Feature	Sets the visibility of thread features in the view. Select the check box to display thread features. Clear the check box to hide them.
Weld Annotations	Associates model weld caterpillars and end fills to the view. Select the check box to get the model weld annotations. Clear the check box to place the view without model weld annotations.
User Work Features	Recovers work features from the model into the view. Select the check box to include the work features. Clearing the check box does not recover them. This setting is used only for initial view placement. To include or exclude work features in an existing view, expand the view node in the Model browser and right-click the model. Select Include Work Features and then specify appropriate work features on the Include Work Features dialog box. Or, right-click a work feature and select Include. To exclude work features from the drawing, right-click the individual work feature and clear the Include check box.
Interference Edges	Enables the visibility of associated drawing views. When selected, associated drawing views are to display both hidden and visible edges that were previously excluded due to an interference condition (press, or interference fit conditions, threaded fasteners in tapped holes where the hole feature is modeled with the minor diameter). This option is enabled only when you edit or create drawing views of assembly or presentation files.
Tangent Edges	Sets the visibility of tangent edges of the selected view. Select the check box to display tangent edges. Clear the check box to hide them.
Foreshortened	Sets the display of tangent edges. Select the check box to shorten the length of tangent edges to distinguish them from visible edges.
Section Standard Parts	Controls the sectioning of standard parts in the drawing view of assemblies. By default, Obey Browser Settings is selected. Section standard parts is Off by default in the drawing browser. The setting can be changed to Always or Never. Never section: Standard parts are never sectioned even when the Section option is turned on in the browser Always section: Standard parts are always sectioned even when turned off in the browser. Obey Browser settings: Defaults to browser setting. Use the current Section option setting that is visible in the browser for assembly views. The section option is only available for assembly views. Note: This setting is disabled for views of parts.
Show Trails	Shows or hides the trails in the selected view, when the source file is a presentation.
Hatching	Sets the visibility of the hatch lines in the selected section view.
Align to Base	Sets the alignment constraint of the selected view to its base view. When the check box is selected, an alignment exists. Clear the check box to break the alignment.
Definition in Base View	Controls the display of detail circles, section lines, and their associated text. Select the option to display the annotations.
Orientation from Base	Specifies camera orientation of a dependent view when base view is rotated or re-oriented. When selected, the dependent view inherits the new orientation from the base view.
Cut Inheritance	Switches on and off the inheritance of a breakout, break, section, and slice cut for the edited view. Select the check box to inherit the corresponding cut from the parent view. Note: The available options are determined by the type of the edited view.
View Justification	Sets the justification of the view. Click the arrow to select Centered or Fixed.

Additional options

Orientation

Sets the view orientation. Select a standard orientation from the list. The list is available only when you create a base view. Click Change View Orientation to specify a custom orientation in the Custom View window. Tip: By default, a parent view and its child views keep the same orientation. To break the orientation inheritance, double-click a child view. Open the Display Options tab in the Drawing View dialog box, and clear the Orientation from Base box.

View/Scale Label		Click Toggle Label Visibility to turn visibility of the view label on or off.
	Scale	When placing a view, sets the scale of the view relative to the part or assembly. When editing a dependent view, sets the scale of the view relative to the parent view. Enter the scale in the box or click the arrow to select from a list of commonly used scales. Note: You can enter a scale that is not on the list. The new scale appears above a line in the list and is available until you close Autodesk Inventor. Tip: Edit the standard settings to customize the list of pre-defined scales. On the ribbon, click Manage tab Styles and Standards panel Styles Editor and then click the current standard. Then add or remove scales in the Preset Values list on the General tab.
		Scale from Base sets the scale of a dependent view to be the same as the scale of its parent view. When selected, the dependent view maintains the same scale as its parent view. To change the scale of a dependent view, clear the check box, and then set the scale Note: If the Scale from Base check box is selected, you cannot change the scale of a dependent view.
	View Identifier	Edits the view identifier string.
		Edits the view label text in the Format Text dialog box.

Style	Sets the display style for the view. To change the display style, click a command. Displays hidden lines in the view. Removes hidden lines from the view. Displays shaded model in the view. Sets the display style of a dependent view to be the same as that of its parent view. When the check box is selected, the dependent view uses the same display style as its parent view. To change the display style, of a dependent view, clear the check box. Note: You can control hidden line visibility after drawing view creation using the Hidden Lines command accessed from the context menu of a component. Click the Hidden Lines to toggle between views. Right-click a component in the browser and select Hidden Lines.
	Enable/Disable Feature Preview Select the check box to preview the drawing view before it is created. Note: The option is selected and unavailable if Show Preview As All Components is selected on the Drawing tab of the Application Options dialog box. If Show Preview As Partial or Bounding Box is selected, the Preview option is available and canceled by default.
	Create projected views immediately after base view creation Make sure the box is checked if you want to create a base view and projected views at the same time. Projected views are relatively positioned to the base view. During the edit, the check box is disabled.
Raster View Only	Select the check box to generate raster drawing views. Raster views are pixel based views that generate much faster than a precise view and are useful for documenting large assemblies. After creation, use the context menu to convert a raster view to a precise view, or a precise view to a raster view. A raster view is framed by a green box in the display. A raster view in the browser is represented by a diagonal red line in the view icon . Some commands are not available in a raster view.