In part and sheet metal models, you can use the Annotation tab to specify the default text strings to indicate bend direction.

When you create drawing views using a template, you can use the Annotation tab to specify annotation options for a variety of drawing views, including flat pattern drawing views, and for drawing view and view annotation captions.

Show detail view borders

Specifies whether borders are shown in detail views.

Retrieve dimensions during view creation

Specifies whether the Retrieve Dimensions command is run when an orthogonal drawing view is created.

Include PMI dimensions from model views

Sets a default on the Drawing View Wizard dialog box to copy product manufacturing information (PMI) dimensions from a model view to a drawing view.

Include PMI annotations from model views

Sets a default on the Drawing View Wizard dialog box to copy product manufacturing information (PMI) annotations from a model view to a drawing view.

Show tube centerlines

Specifies whether tube centerlines are displayed in drawing views. You can override this setting for views as they are created with the Show tube centerlines check box on the Drawing View Options page of the Drawing View Wizard.

Show flowlines

Displays the flow lines in a drawing view of an exploded assembly.

Exploded flowline style

Sets the style for exploded assembly flow lines.

Show boundary edges

Displays edges where the drawing view border overlaps the model.

For more information, see Drawing view cropping.

Boundary edges style

Sets the style for cropping and other boundary edges.

Show threads in Section Only section views

Sets the default display for threaded cylinders when the cut is along the axis of the hole shown in paper-thin section drawing views.

Caption

Show sheet number if parent annotation (e.g. cutting plane) and derived view (e.g. section view) do not reside on the same sheet

Displays a cross-reference between the sheet the view annotation is on and the sheet the drawing view is on. When either is moved to a different sheet, the following information is displayed in the drawing view captions:

• The annotation sheet number is displayed with the derived drawing view.

• With the view annotation, the derived drawing view sheet number is displayed.

Note:

This option only works as described when you define drawing view captions using property text. In this case: %LN and %VN must be added to the caption text, and the appropriate property text must be added to the Annotation Sheet Number and View Sheet Number edit boxes.

If the views are moved again so that they are on the same sheet, then the sheet cross-reference information is not displayed on the drawing.

Show drawing view scale if different from sheet scale

When a drawing view is created that has a different scale than the sheet scale, automatically displays the drawing view scale in the caption.

Note:

This option only works as described when you define drawing view captions using property text. In this case, %VS must be added to the caption text, and the appropriate property text must be added to the View Scale edit box.

If the drawing view scale subsequently changes so that it matches the sheet scale, then the scale value is not shown in the caption.

Show rotation angle if drawing view is rotated

If a drawing view is rotated after placement, displays the rotation angle in the drawing view caption. Drawing views may be rotated using the Rotation command or by changing the Rotation angle value on the General page of the Drawing View Properties dialog box.

Note:

This option only works as described when you define drawing view captions using property text. In this case, %VR must be added to the caption text, and the appropriate property text must be added to the Angle of Rotation edit box.

If the drawing view is rotated back to zero degrees, the rotation angle is not shown.

Auto-Naming of View Annotations

Specifies the order that is used to assign names automatically to detail envelopes, cutting plane lines, viewing plane lines, and datum frames. They also specify the characters used to generate the names that appear in view annotation captions and in datum frame annotations.

Specify Annotation Letters

Opens the Specify Annotation Letters dialog box, where you define the sequence of letters and numbers for generating view annotation and datum frame labels automatically.

To learn how, see the Help topic, Define annotation labels.

Follow object creation sequence

Names the view annotations automatically based on the natural order in which they are created.

Follow defined object sequence

Names the view annotations automatically based on the priority order assigned in the Define Object Sequence dialog box.

Define Sequence

Opens the Define Object Sequence dialog box, where you prioritize the order for assigning the view annotation and datum frame labels defined in the Specify Annotation Letters dialog box.

Warning:

If viewing planes, cutting planes, detail envelopes, or datum frames exist in the document, then switching from Follow object creation sequence to Follow defined object sequence renames all of the existing annotation objects. This operation cannot be undone.

Sheet Metal Flat Pattern

Show bend centerlines

Displays the bend centerlines on drawing views of sheet metal part flat patterns.

Bend up centerline style

Sets the style for centerlines on bends in the up direction.

Bend down centerline style

Sets the style for centerlines on bends in the down direction.

Bend up string

Specifies a custom string to display when the bend direction is up. The default string is Up.

This text string can be specified independently in part and sheet metal models, and on flat pattern drawing views.

Bend down string

Specifies a custom string to display when the bend direction is down. The default string is Down.

This text string can be specified independently in part and sheet metal models, and on flat pattern drawing views.

Bend unknown string

Specifies a custom string to display when there is no associated sheet metal flat pattern. The default string is Undefined.

This option applies only to bends displayed in part and sheet metal models.

Derive bend direction from drawing view

Allows the flattened drawing view to determine bend direction rather than the model. (By default, bend direction is derived from the face that is designated the top face when a sheet metal part is flattened.)

Tip:

Use the Derive bend direction from drawing view option to keep the bend direction properly aligned with the drawing view that you place.

• When this box is checked, the bend direction shown in a top drawing view will be the opposite of that shown in a bottom drawing view.

• When this box is checked, the bend up and bend down centerline styles also are applied based on the drawing view bend direction.

• When this box is unchecked, the bend direction will be the same for both top and bottom views.

Show deformation feature origins

Displays the feature origins of sheet metal part flat patterns.

Origin edge style

Sets the style for feature origins.

Show deformation feature profiles

Displays the feature profiles of sheet metal part flat patterns.

Profile edge style

Sets the style for feature profiles.