ViewBase

NOTES

• This command is valid in model space only .
• Use the Tab key to select obscured entities.
• The GENERATEASSOCVIEWS (Generate associative drawings) system variable enables associative dimensions for generated views, as a result they are updated automatically when the 3D model changes.
• The GENERATEASSOCATTRS (Generate associative attributes) system variables controls the generation of associative data on 3D solids during modeling. When ON, 3D solids contain associative data upon creation. This allows VIEWBASE to generate drawings in which dimensions and tags are updated automatically when the 3D model has been modified.

Select objects

Selects the entities in model space from which to generate the drawing views in a layout tab.

Entire model

Select all the 3D entities in model space.

preseTs

Specifies the types of generated drawings and their placement in the layout; displays the Drawing View Presets dialog box; see below.

The selected preset is saved through the DRAWINGVIEWPRESET system variable.

Special views

Select a style of exploded representations, if any exist in the drawing;
prompts you:

Select view [Exploded view/Unfolded view/Back] <Back>: - (enter an option:)

• Exploded view -displays a dialog box:
  
  From the drop-down list, choose a style for the exploded representation. Prompts you:

  Enter new or existing layout name to make current <LayoutName>: (Enter the name of a new or existing layout, or press Enter to accept the current layout)

  The command switches to the layout tab, prompts you:

  Select position for base view [Scale/Hidden lines/Tangent lines/trailiNg lines/Orientation/Projection type/Isometric geometry/sElect/eXit] <eXit>:
  • trailiNg lines - controls the visibility of trailing lines; prompts you:
    Show trailing lines [Yes/No]: - (enter an option);
• Unfolded view - prompts you:
  Select a solid with associated unfolded view [Back/selection options (?)]: - (Select one or more 3D solids in model tab, or press Enter to select all of them)
• Back - returns to the previous prompt.

To create exploded views, use the BMEXPLODE command; the model must have inserts of mechanical components to use this command.

selection options (?)

Selects one or more entities through a variety of selection methods, see Select.

Scale

Sets the Scale property of the paper space viewports for the various views; prompts you:

Adjust view scale [fit 4 views/fit 9 views/fit 5 views/fit 10 views/Standard scales/Custom scales] <fit 4 views>: - (enter an option:)

• fit 4 views - adjusts the scale is adjusted to fit the four standard orthographic views: Front, Top, Left, Right. The Front view (base view) is defined by the Orientation option.
• fit 9 views - adjusts the scale to fit five orthographic views and four isometric views.
• fit 5 views - adjusts the scale to fit five orthographic views: Front, Top, Left, Right, Back.
• fit 10 views - adjusts the scale to fit six orthographic views and four isometric views. <
• Standard scales - displays the scale list as maintained by the ScaleListEdit command; select a scale from the list.
• Custom scales - prompts you to type a scale in the command bar.

Hidden Lines

Controls the visibility of hidden lines; prompts you:

Show hidden lines [Yes/No] - (enter an option:)

• Yes - displays hidden lines in the section view
• No - turns off hidden lines

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

Tangent Lines

Toggles whether tangent edges between tangent faces are created. Visible tangent edges are created on the BM_Tangent_Visible layer. Hidden tangent edges are created on the BM_Tangent_Hidden layer. Prompts you:

Enable tangent edges on basic views? [Yes/No] <No> - (enter an option:)

No - does not display tangent lines:

Yes - displays tangent lines:

Tangent edges are always created for isometric views. Freeze or switch off the display of the BM_Tangent_Visible layer to hide tangent edges in isometric views.

Orientation

Defines the base view. Rotates the 3D model so that the main view is projected on the vertical projection plane (V.P.).

Prompts you:

Select orientation [Front/bAck/Left/Right/Top/Bottom/Current] <Front>: - (enter an orientation to change the base view.)

Projection type

Defines the layout of the views; prompts you:

Select the projection type [First angle/Third angle] <First angle> - (enter a projection type:)

• First angle - also known as European projection:

• Third angle - also known as American projection:

The default projection type depends on the value of the MEASUREMENT variable:

• 0 - (Imperial) generates the third angle projection
• 1 - (Metric) generates the first angle projection

Isometric Geometry

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

Create isometric views as [2D views/3D views] <2D views> - (enter an option:)

• 2D views - draws isometric views as 2D drawings:
  
  
• 3D views - draws isometric views as 3D solids with the Conceptual visual style applied.
  
  

Select

Selects additional entities to include or exclude; prompts you:

[Remove/Entire model/Layout/selection options (?)] <Layout>: - (enter an option:)

• Remove - removes entities from drawing views
• Entire model - includes all entities from model space in the drawing views
• Layout - opens the previous layout with updated drawing views

Select position for projected view

Depending on the position of the cursor with respect to the base view one of five orthogonal views (top, left, right, back and bottom) and four isometric views can be inserted. The views are aligned automatically depending on the selected projection type (see above).

Tap the Ctrl key to toggle alignment on and off; when off, you can place the current view in any location.

eXit

Concludes the command.

When the GENERATEASSOCVIEWS variable is On, associative dimensions are updated automatically when the 3D model is modified.

DRAWINGVIEWQUALITY variable defines the quality of drawing views.

Select a preset view arrangement:

1. Click the Preset droplist

2. Choose an option

• None - no preset affects the views generated
• Architectural Views - generates
  • Five standard views: Front, Right, Back, Left (used for elevations) and Top views
  • Three section views: two horizontal sections (for plans) and 1 vertical section
• Mechanical Views - generates
  • Three standard views: Front, Top and Left (first angle projection) or Right (third angle projection)

The layout of the mechanical views is controlled by the projection type: first or third angle. The current projection type is saved in the PROJECTIONTYPE variable.

Sets the default scale factor for the drawing views:

1. Click the View Scale droplist

2. Select a scale factor.

The scale list can be edited by the ScaleListEdit command.

1. Click the Hidden Lines droplist

2. Choose Visible or Invisible.

Sets the default for Tangent Lines in drawing views:

1. Click the Tangent Lines droplist

2. Choose Visible or Invisible.