ViewBase

NOTE

The GENERATEASSOCVIEWS system variable controls whether ViewBase produces 2D views which are persistently associated with the source 3D model.

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

Select objects

Allows to compose a selection set of objects to be included in the process. Repeatedly hit the TAB key to iterate through the entities on different nesting levels.

Presets

Allows to select a preset, which controls the number of generated drawing views and their placement in the layout.

The selected preset is saved through the DRAWINGVIEWPRESET system variable.

Displays a dialog box:

Click the Preset button to select a preset. The options are:

• None

• Architectural Views: generates Front, Right, Back, Left (elevations) and Top views and 3 section views: two horizontal sections (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 is controlled by the projection type: first or third angle. The current projection type is saved through the PROJECTIONTYPE system variable.

Click the View Scale button, then select a scale. The scale list can be edited by the ScaleListEdit command.

Scale

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

Prompts you:

Adjust view scale [fit 4 views/9 views/5 views/10 views/Standard scales/Custom] <fit 4 views>:

Select an option:

• fit 4 views: The scale is adjusted to fit 4 orthographic views: Front (*), Top, Left, Right.

• 9 views: The scale is adjusted to fit 5 orthographic views and 4 isometric views.

• 5 views: The scale is adjusted to fit 5 orthographic views: Front (*), Top, Left, Right, Back.

• 10 views: The scale is adjusted to fit 6 orthographic views and 4 isometric views.

• 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.

(*) The Front view (base view) is defined by the Orientation option.

Hidden Lines

Allows to control the creation of hidden lines. Hidden lines are created on the BM_Hidden layer.

Prompts you:

Enable hidden lines on basic views? [Yes/No] <Yes> - choose an option.

Tangent Lines

Defines whether tangent edges between tangent faces are created or not.

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>:

NO :

Yes :

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 main 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] <Front>:

Select the base view.

Projection type

Defines the layout of the views.

Prompts you:

Select the projection type [First angle/Third angle] <First angle>:

First Angle or European projection:

Third Angle or American projection:

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

• 0 (Imperial): Third Angle projection.

• 1 (Metric): 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>:

• 2D : Isometric views are 2D drawings.
  
  

• 3D : Isometric views are 3D solids. The viewport has the Conceptual visual style applied.
  
  
  Optionally, choose a different visual style for the viewport in the Properties Bar .
  
  

Select

Allows to select additional entities to be included or entities to be removed. Repeatedly hit the TAB key to iterate through the entities on different nesting levels, which allows to select solids in nested components.

Prompts you:

Select objects to add to set or [Remove/Entire model/Layout] <Layout>:

Select entities to add to drawing views or select:

• Remove: select entities to be removed from the drawing views

• Entire model: all entities from model space will be included 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. Hit the CTRL key to toggle the alignment On/Off. If TIPS = ON in the Status Bar, the TIPS widget displays, indicating the current status of the view alignment:

• Alignment ON: Views align with respect to the base view.

• Alignment OFF: Views can be inserted freely.

Done

Concludes the command.