ViewSection

Type

Allows to control the shape of the section plane.

Prompts you:

Select type [Full/Half/Offset/Aligned] <Full>:  

Select an option.

• Full (): The section line defines an infinite plane cutting through the entire model.

• Half (): The section line defines a half-plane cutting part of the model.
  Prompts you:
  Specify start point of section line or [Type] <Type>: Specify a point (1).
  Specify next point of section line [Done] <Done>: Specify a point to define the limit of the half plane (2).
  Specify next point of section line [Done] <Done>: Specify a point to define the view direction (3).
  The position of the third point  controls whether the part of the model that is not cut displays (left) or not (right).
  
  

• Offset (): The section line defines a series of cutting regions located on different offsets from each other. You have to chose Done from the option menu to complete the section line.

• Aligned (): the section line defines a polyline, where every segment defines a cutting region. The resulted section will have the length equal to the sum of the lengths of cutting regions. You have to chose Done from the option menu to complete the section line.

Scale

Sets the Scale property of the paper space viewports for the various views.

Prompts you:

Adjust view scale [Standard scales/Custom/from Parent]:

Select an option:

• Standard scales: Displays the scale list as defined by the ScaleListEdit command.
  Select a scale in the list.

• Custom: Prompts you to type a scale in the command bar.

• From Parent: Sets the scale of the section equal to the scale of the parent viewport.

Hidden Lines

Allows to control the visibility of hidden lines.

Prompts you in the command bar:

Show hidden lines [Yes/No/from Parent]:

• Yes: Displays hidden lines in the selected drafting viewports.
  If the BM_Ortho_Hidden and BM_Isometric_Hidden layers are OFF or Frozen, hidden lines will not display.

• No: Switches the display of hidden lines in the selected drafting viewports off.

• From Parent: Copies the Hidden Lines property from the parent viewport.

Tangent Lines

Allows to control the display of tangent edges between a flat and a curved face (e.g. a filleted edge).

Prompts you:

Show tangent lines [Yes/No]:

• Yes: Tangent lines display. This is the default setting.
  

• No: Tangent lines are suppressed.
  

Anchor

Allows to control how to position the view inside the viewport in an update operation, when the extents (= bounding box) of the 3D geometry has been changed.

Prompts you:

Anchor view on paper space? [Yes/No]:

• Yes: The center of the viewport is anchored. The size of the viewport grows or shrinks around its center point.

• No: The position of the unchanged geometry is fixed. This is the default behavior.

The AUTOVPFITTING system variable controls whether the size of the viewport is adjusted automatically to fit the current extents of the 3D geometry. By default AUTOVPFITTING = ON.

Isometric Style

Defines the style for the isometric views: rendered 3D view or 2D drawing.

Prompts you:

Enable conceptual visual style for isometric views? [Yes/No] <No>:

• Yes: Isometric views use the Conceptual visual style.
  
  
  Optionally, choose a different visual style for the viewport in the Properties Bar.
  
  

• No: Isometric views are 2D drawings.
  
  

Annotation

Controls the annotation of the detail view or section view.

Prompts you:

Select annotation [Identifier/Label]:

• Identifier: Prompts you to specify the view detail identifier:
  Specify the identifier <A>: Enter a name for the view detail.

• Label: Prompts you to display of the view detail label.
  Show view label [Yes/No]:  Choose an option.

Depth

Specifies the view depth of a section view.

Prompts you:

Choose depth mode [Full/Custom]:

• Full: The view depth is set to the extents of the model (= maximum view depth).

• Custom: Allows to limit the view depth.
  Prompts you:
  Enter depth distance:
  Type a positive value then press Enter.
  or
  Define the view depth dynamically using the pointing device: a line, indicating the view depth, displays dynamically. Click a point.

Projection

The command prompts you:

Select projection method [Normal/Orthogonal]:

Select the desired method:

• Normal: Creates the section as a union of projections of every cutting region (each segment of a the section polyline) in its normal direction.

• Orthogonal: Creates the section in normal direction of the first section region (first segment of the section polyline).