2D Sketching in Drawings
You can create drawing geometry using 2D sketched geometry only, without
reference to existing models or assemblies. This sketched geometry can
be controlled by relations (collinear, parallel, tangent, and so on),
as well as parametric dimensions.
Sketch tools and sketch relations work the same way in a drawing document
as they do in a part or assembly document. The only difference is that
instead of sketching on model planes or faces, you sketch on the drawing
sheet or in an active view.
When you drag a sketch point
in a drawing, it snaps or infers to other sketches, drawing views, blocks,
and items in the sheet format.
If you add sketch entities
to a drawing view, the border automatically resizes to include these items.
Grid
To toggle display a grid, right-click the active drawing sheet and select
Display Grid.
Specify grid spacing, line style, etc. in Tools,
Options, Document
Properties, Grid/Snap.
Sketch Entity Alignment
You can constrain sketch entities to geometry in multiple drawing views.
Use relations as in sketches. In this
example, a sketch point in the top view is coincident with the virtual
sharp of the part, and the sketched line in the bottom view is coincident
with the view's geometry and the sketch point in the top view.
Empty View
You can create an empty drawing view to contain sketch geometry. When
this view is activated, all sketch geometry added belongs to the view.
The sketch geometry can then be scaled, moved, and deleted as a group
while still retaining the editability of the individual sketch entities.
To create an empty drawing view:
Click Empty View
(Drawing toolbar) or Insert, Drawing View,
Empty.
Click to place the view in the graphics area.
Importing Sketch Geometry
You can import DXF/DWG files into a SolidWorks drawing. Then you can
insert that geometry into a sketch to create model features in a part.
For more information, see DXF/DWG Files(*.dxf,*.dwg).
2D Emulator
The SolidWorks software includes an add-in
application that allows you to create sketch entities by entering commands
in text form. For more information, see SolidWorks 2D Emulator.
Related Topics
Sketching
in SolidWorks
Geometric
Relations