The options available depend upon whether the model is assembly, part, or sheet metal.
Designed part
Specifies that you want to create a drawing view of the part as designed. This option is only available for Part and Sheet Metal files.
Simplified part
Specifies that you want to create a drawing view of the simplified version of a part. This option is only available for Part and Sheet Metal files. It is disabled if a simplified model does not exist.
Flat pattern
Specifies that you want to create a drawing view of the flattened sheet metal part. This option is only available for sheet metal files that also contain the flattened model in the file.
PMI model view
For a part or sheet metal model, lists the names of available PMI model views that can be used to generate a drawing view.
.cfg, PMI model view, or Zone
For an assembly model, lists the names of available display configurations, 3D PMI model views, and zones that can be used to generate a drawing view.
– Indicates a display configuration.
– Indicates a 3D PMI model view.
– Indicates a zone.
Example:
You can hide parts or weld beads in the assembly document, save the display configuration to a name you define, then use that display configuration when creating the drawing view. For more information, see the Using display configurations Help topic.
If you select a PMI model view created with the View command, then the model view controls the display states of parts in an assembly.
If you used the Create Zone command to define a rectangular volume of space based on one or more assembly components, then you can create a drawing view of the components that are contained within the boundary of the zone.
Include PMI dimensions from model views
Set this option to retrieve the PMI dimensions associated with a model view you have selected in the PMI Model View list (for part/sheet metal models) or in the Configuration and PMI Model View list (for assembly models). By default, the copied PMI dimensions are associative to the drawing view.
Include PMI annotations from model views
Set this option to retrieve the PMI annotations associated with a model view you have selected in the PMI Model View list (for part/sheet metal models) or the Configuration and PMI Model View list (for assembly models). By default, the copied PMI annotations are associative to the drawing view.
Use simplified assemblies
Specifies that you want to create a drawing view of an assembly using the simplified assembly representation. This option is not available for assembly zones.
For all subassemblies
Specifies that you want to create a drawing view that shows all the subassemblies as simplified for which a simplified representation exists. This option is only available for Assembly files.
Based on configuration
Specifies that you want to create a drawing view that displays the subassemblies as simplified or as designed based on the configuration you select. This option is only available for Assembly files.
For top assembly
Specifies that you want to create a drawing view that displays only the top level assembly as simplified. This option is only available for Assembly files.
Use simplified parts
Specifies that you want to create a drawing view of an assembly with simplified models. This option is only available for assembly files.
For all parts
Specifies that you want to create a drawing view that shows all the parts as simplified for which a simplified model exists. This option is only available for assembly files.
Based on configuration
Specifies that you want to create a drawing view that displays the parts as simplified based on the configuration. This option is only available for assembly files.
Create draft quality drawing views
Quickly creates draft-quality drawing views of an assembly. You can use draft quality views as input for principal views, auxiliary views, cutting planes, and broken-out section views. You can also add balloons to draft quality views and create parts lists from them. This option is only available for Assembly files.
To place a 3D cutaway/section view on a drawing sheet, the Create Draft Quality Drawing Views option must be set. After placing a drawing view, use the Sections page on the Drawing View Properties dialog box to select and display the 3D cutaway/section view on the drawing sheet.
View quality
Specifies the quality or resolution when a draft quality drawing view is created or updated. The resolution defines the pixel range box used to display the draft quality view. Three is the highest value and provides the best setting. The quality value is saved with the drawing view.
You can modify the Draft View Quality value on the General page of the Drawing View Properties dialog box after placing the drawing view. If you modify the value there, the drawing view will go out-of-date.
This option is only available when Create Draft Quality Drawing Views is also checked.
Activate parts for dimensioning
Activates (loads into memory) the parts in the assembly so that you can use them for dimensioning and other operations that require precision. You cannot dimension pre-v17 pictorial views. This option is only available when Create Draft Quality Drawing Views is also checked.
Show tube centerlines
Displays tube centerlines in the drawing view(s). This setting overrides the Show Tube Centerlines check box on the Edge Display page of the Options dialog box. This option is not available for Sheet Metal and Weldment files.
Show assembly features
Specifies whether assembly features created in the Assembly environment are shown in the drawing view. This option applies only to material removal features such as holes, chamfers, and cutouts. When this box is checked, these types of assembly features are displayed in the drawing view even if the Use Simplified Parts box is also checked. This option is only available for Assembly files.
To control the display of material addition features, such as fillet welds and protrusions, you can use the options on the Display page of the Drawing View Properties dialog box. You can also define a display configuration in the assembly with material addition features hidden, then use the display configuration when placing a drawing view of the assembly.
Derive "Display as Reference" from assembly
Specifies that the occurrence properties defined in the assembly document determine whether the occurrence is displayed as a reference part. Reference parts are displayed using a different line style you can define. You can use the Occurrence Properties command on the Assembly PathFinder shortcut menu to specify that an assembly occurrence is displayed as a reference part in a drawing. You can use the Edge Display page on the Solid Edge Options dialog box to specify the reference part edge display style you want to use.
Machined view
Specifies that you want to create a drawing view of a machined view of a weldment. This option is only available for weldment files (.pwd).
Welded view
Specifies that you want to create a drawing view of a welded view of a weldment. This option is only available for Weldment files (.pwd).
Assembly view
Specifies that you want to create a drawing view of an assembly view of a weldment. This option is only available for Weldment files (.pwd).
Show hidden edges in:
Orthographic views
Displays the hidden edges on parts in orthographic part views.
Pictorial views
Displays the hidden edges on parts in pictorial part views.
Show tangent edges in:
Orthographic views
Displays the tangent edges on parts in orthographic part views.
Pictorial views
Displays the tangent edges on parts in pictorial part views.
Show edges of hidden parts in:
Orthographic views
Displays the parts that are hidden by other parts in orthographic part views. The edges are displayed using the hidden edge line style. This option is only available for Assembly and Weldment files.
Pictorial views
Displays the parts that are hidden by other parts in pictorial part views. The edges are displayed using the hidden edge line style. This option is only available for Assembly and Weldment files.
Advanced
Displays the Advanced Edge Display Options dialog box.
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