Generates associative orthographic and isometric views of 3D models in paper space layouts.
NOTES |
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Accessing the Command
command bar: viewbase
transparent: 'viewbase
menu bar: Model | Drawing Views | Generate Drawing Views
toolbar: Drawing Views | Generate Drawing Views
ribbon (Mechanical workspace):
- Home | Drawing Views | Generate Drawing Views
- Annotate | Drawing Views | Generate Drawing Views
: ViewBase
Prompts you in the command bar:
Preset: "None", View scale: "Adapt to paper size"
Select objects or [Entire model/preseTs/Special views/selection options (?)] <Entire model>: (Select one or more 3D solids in model tab, or else press Enter to select all of them; or else enter an option)
Enter new or existing layout name to make current <LayoutName>: (Enter the name of a new or existing layout, or else press Enter to accept the current layout)
The command switches to the layout tab:
Select position for base view [Scale/Hidden lines/Tangent lines/Orientation/Projection type/Isometric geometry/sElect] <eXit>: (Pick a point at which position the base view, or else enter an option)
Select position for projected view [eXit] <eXit>: (Move the cursor left, right, above or below the base view to create other views, and click; continue until the final view is inserted or press Enter to finish early)
Command Options
Option |
Description |
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:)
To create exploded views, use the bmExplode command; before this command can be used, the drawing must have inserts of mechanical components. |
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:)
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Hidden Lines |
Controls the visibility of hidden lines; prompts you: Show hidden lines [Yes/No] - (enter an option:)
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:)
The default projection type depends on the value of the MEASUREMENT variable:
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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:)
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Select |
Selects additional entities to include or exclude; prompts you: [Remove/Entire model/Layout/selection options (?)] <Layout>: - (enter an option:)
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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. 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. |
NOTES |
When the GENERATEASSOCIVIEWS variable is on, associative dimensions are updated automatically when the 3D model is modified. DRAWINGVIEWQUALITY variable defines quality of drawing views. |
Drawing View Presets Dialog Box
To access this dialog box, enter the preseTs option:
Dialog Box Option |
Description |
Preset |
Select a preset view arrangement:
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. |
View Scale |
Sets the default scale factor for the drawing views:
The scale list can be edited by the ScaleListEdit command. |
Hidden Lines | Sets the default setting for hidden lines in drawing views:
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Tangent Lines |
Sets the default for Tangent Lines in drawing views:
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Related Commands
Flatshot - creates a hidden line representation of 3D solids in model space.
MvSetup - creates multiple paper space viewports; aligns, rotates and scales paper space viewports. In model space the command creates a rectangle, representing a paper sheet with respect to a specified scale.
Solprof - creates a hidden line representation of 3D solids in a layout viewport.
ViewDetail - creates a detail view of a portion of a standard generated drawing at a larger scale.
ViewDetailStyle - allows to specify the visual format of detail views and detail symbols.
ViewEdit - allows changing the scale and the hidden line visibility of drawing views.
ViewExport - Exports the content of drawing views obtained by ViewBase and ViewSection to the Model Space of the drawing or to a new drawing.
ViewProj - generates additional projected views from an existing drawing view.
ViewSection - creates a cross section view based on a standard drawing view generated by the VIEWBASE command in a paper space layout.
ViewSectionStyle - allows to specify the visual format of section views and section lines.
ViewUpdate - updates a selection of drawing views or sections when VIEWUPDATEAUTO = 0.