ViewSection

NOTE

Select drawing view

Selects the drawing view to generate the section from - click inside a drawing view.

Specify start point of section line

Specifies one end of a section line - pick a point in the layout.

Specify next point of section line

Specifies the second point of the section line. Prompts you:

Specify next point of section line [Done] <Done> - (Enter an option.)

• Pick another point to create a jogged section line
• Enter Done to end the draw section process

The command repeats so that you can draw sections lines with jogs.

Select type

Control the shape of the section plane. Prompts you:

Select type [Full/Half/Offset/Aligned] <Full> - (Enter an option:)

1. Full - section line defines an infinite plane that cuts through the entire model.

2. Half - section line defines a half-plane that cuts part of the model. Prompts you:

3. Specify start point of section line or [Type] <Type> - (pick a point - #1 in the figure below.)

4. Specify next point of section line [Done] <Done> - (pick another point to define the limit of the half plane - #2 in the figure below.)

5. Specify next point of section line [Done] <Done> - (pick the point that defines the view direction - #3 in the figure below.) The position of the third point determines 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. Enter Done 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. Enter Done to complete the section line.

Select position for section view

Specifies the location of the section view:

• As you move the cursor, the section view stays perpendicular to the section line.
• To place the section view anywhere on the sheet, hit the Ctrl key to turn off alignment.

Scale

Sets the scale of the section view. Prompts you:

Adjust view scale [Standard scales/Custom/from Parent] - (Enter an option:)

• Standard scales - displays the list of scale factors defined by the ScaleListEdit command. Prompts you:
  Enter the scale number <1> - (Enter a number from the list displayed by the program.)
• Custom - prompts you to enter a scale in the command bar:
  Enter scale <1.000> - (Enter a scale factor.)
• from Parent - sets the scale of the section view equal to the scale of the parent viewport.

Hidden lines

Allows you to control the visibility of hidden lines. Prompts you:

Show hidden lines [Yes/No/from Parent] - (Enter an option:)

• Yes - displays hidden lines in the section view
• No - turns off hidden lines
• from Parent - uses the same hidden line setting as the parent view

When the BM_Ortho_Hidden and BM_Isometric_Hidden layers are off or frozen, hidden lines do not display.

Tangent lines

Controls the display of tangent edges, which appear in the transition from a flat face and a curved face. Prompts you:

Show tangent lines [Yes/No] - (Enter an option:)

• Yes - displays tangent lines:
  

• No - does not display tangent lines:
  

anChor

Determines how the viewport changes relative to the section. Prompts you:

Anchor view on paper space? [Yes/No] - (Enter an option:)

• Yes - the center of the viewport is anchored so that the viewport grows and shrinks around its center point

• No - the position of the geometry is fixed

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

Geometry

Selects the visual style for the section view. Prompts you:

Choose geometry type [2D/3D] - (Enter an option:)

• 2D - section view uses the 2dWireframe visual style

• 3D - section view uses a rendered visual style. This is Conceptual by default. Use the Properties panel to choose a different visual style:
  
  

Annotation

Determines the annotations to use. Prompts you:

Select annotation [Identifier/Label] - (Enter an option:)

• Identifier - specifies the view detail identifier. Prompts you:
  Specify the identifier <A> - (Enter a name for the view detail)

• Label - toggles the display of the view detail label. Prompts you:
  Show view label [Yes/No] - (Press Y or N.)

Depth

Specifies the view depth of a section view. Prompts you:

Choose depth mode [Full/Custom] - (Enter an option:)

• Full - sets the depth to the extents of the model (maximum view depth)

• Custom - limits the view depth. Prompts you:
  Enter depth distance - (Type a positive value or move the cursor to define the view depth dynamically.)

Projection

Determines how the section is projected. Prompts you:

Select projection method [Normal/Orthogonal] - (Enter an option:)

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

• Orthogonal - draws the section in the normal direction of the first section region (the first segment of the section polyline).

Allows you to rotate the drawing view viewport but does not rotate the frame. Prompts you:

Select first point of segment: (Pick a point or enter x,y coordinates)
Select second point of segment: (Pick a point or enter x,y coordinates)
Select orientation [Horizontal/Vertical/Custom angle]:

• Horizontal: rotates a segment horizontally.
• Vertical: rotates a segment vertically.
• Custom angle: allows you to specify the angle of alignment. Prompts you:
  Specify the angle: enter the rotation angle or pick the rotation point.
  Second point: enter an angle or pick a point.

• The GENERATEASSOCVIEWS system variable controls whether VIEWSECTION produces 2D views. These are associated with the source 3D model.

• If GENERATEASSOCIVIEWS is ON, associative dimensions are updated automatically when the 3D model is modified.

• If the Sectionable property of a mechanical component is OFF, the component appears non-sectioned in the section views of the Full section type.