Draft Shape2DView
Draft Shape2DView |
Menu location |
---|
Modification → Shape 2D view |
Workbenches |
Draft, Arch, Part, TechDraw |
Default shortcut |
None |
Introduced in version |
- |
See also |
None |
Description
The Draft Shape2DView tool produces a 2D projection from a selected 3D solid object such as those created with the Part, PartDesign, and Arch Workbenches.
The resulting projection is a Draft object and is placed in the 3D view. This object can be displayed on a TechDraw Workbench page, using the TechDraw DraftView tool. Alternatively, TechDraw has its own tools to create projected views, the TechDraw View and TechDraw ProjectionGroup tools; however, these tools are meant for preparing technical drawings, so they create the views only in the drawing page, and not in the 3D view.
Projection of solid shapes into the XY plane
Usage
- Rotate the view so it reflects the direction of the desired projection. For example, a top view will project the object on the XY plane.
- Select a 3D object.
- Press the Draft Shape2DView button. If no object is selected, you will be invited to select one.
The projected object will be created below the selected object, lying on the XY plane. It's position can be changed by changing its properties. The projection direction can also be changed after creation with the property editor.
Note: If the selected object is an Arch SectionPlane, the projection will use the contents and direction of that Section plane; in this case, the "Projection" property will be ignored.
Options
There are no options for this tool. Either it works with the selected object or not.
Properties
- DataProjection: specifies the direction of the projection as a vector. For example, (0,0,1) is a projection looking through the Z axis, which would be projected on the XY plane; (1,0,0) is a projection looking through the X axis, which would be projected on the YZ plane; (0,1,0) is a projection looking through the Y axis, which would be projected on the XZ plane. The values can also be negative, in which case the direction of projection is inverted.
- DataProjection Mode: it can be "Solid", "Individual Faces", "Cutlines", "Cutfaces" and "Solid faces" (introduced in version 0.20).
- The default projection is "Solid", which projects the entire selected shape.
- If only some faces of the base object are selected, the "Individual Faces" mode will project only those faces.
- If the selected object is an Arch SectionPlane, the "Cutlines" mode will project only the edges being cut by the section plane.
- If the selected object is an Arch SectionPlane, the "Cutfaces" mode will display the cut areas of solids as faces.
- If "Solid faces" is selected, the projection will be obtained by cutting all individual faces one by one. This is useful when the "Solid" method gives wrong results.
- DataIn Place: if it is
true
, together with "Cutlines" or "Cutfaces" modes, the resulting projection will appear co-planar with the Arch SectionPlane. introduced in version 0.17 - DataHiddenLines: if it is
true
it will show the hidden lines of the projection. - DataTessellation: if it is
true
it will perform tessellation of ellipses and splines, that is, it will represent curves with very fine line segments.
- Note: this may be computationally intensive if DataSegment Length is very small.
- DataSegment Length: specifies the size in millimeters of linear segments if DataTessellation is
true
.
- Note: set a larger value first, and then change it to a smaller value to get better resolution.
- DataVisible Only: if it is
true
the projection will be recomputed only if it is visible.
Scripting
See also: Autogenerated API documentation and FreeCAD Scripting Basics.
The Draft Shape2DView tool can be used in macros and from the Python console by using the following function:
Shape2DView = makeShape2DView(baseobj, projectionVector=None, facenumbers=[])
- Creates
Shape2DView
as a projection of the givenbaseobj
.- If
facenumbers
is given, it is a list of face numbers to be considered for the projection.
- If
- If a
projectionVector
is given, it is used; otherwise the default projection is along the Z axis.
The ProjectionMode
attribute needs to be overwritten with the desired mode, which can be "Solid"
, "Individual Faces"
, "Cutlines"
, or "Cutfaces"
.
Example:
import FreeCAD as App
import Draft
doc = App.newDocument()
box = doc.addObject("Part::Box", "Box")
box.Length = 2300
box.Width = 500
box.Height = 1000
shape1 = Draft.make_shape2dview(box)
shape2 = Draft.make_shape2dview(box, App.Vector(1, -1, 1))
shape3 = Draft.make_shape2dview(box, App.Vector(-1, 1, 1), [0, 5])
shape3.ProjectionMode = "Individual Faces"
doc.recompute()
- Drafting: Line, Polyline, Fillet, Arc, Arc by 3 points, Circle, Ellipse, Rectangle, Polygon, B-spline, Cubic Bézier curve, Bézier curve, Point, Facebinder, ShapeString, Hatch
- Annotation: Text, Dimension, Label, Annotation styles, Annotation scale
- Modification: Move, Rotate, Scale, Mirror, Offset, Trimex, Stretch, Clone, Array, Polar array, Circular array, Path array, Path link array, Point array, Point link array, Edit, Subelement highlight, Join, Split, Upgrade, Downgrade, Wire to B-spline, Draft to sketch, Set slope, Flip dimension, Shape 2D view
- Draft Tray: Select plane, Set style, Toggle construction mode, AutoGroup
- Snapping: Snap lock, Snap endpoint, Snap midpoint, Snap center, Snap angle, Snap intersection, Snap perpendicular, Snap extension, Snap parallel, Snap special, Snap near, Snap ortho, Snap grid, Snap working plane, Snap dimensions, Toggle grid
- Miscellaneous: Apply current style, Layer, Manage layers, Add a new named group, Move to group, Select group, Add to construction group, Toggle normal/wireframe display, Create working plane proxy, Heal, Show snap toolbar
- Additional: Constraining, Pattern, Preferences, Import Export Preferences, DXF/DWG, SVG, OCA, DAT
- Context menu:
- Layer container: Merge layer duplicates, Add new layer
- Layer: Activate this layer, Select layer contents
- Text: Open hyperlinks
- Wire: Flatten
- Working plane proxy: Write camera position, Write objects state
- Getting started
- Installation: Download, Windows, Linux, Mac, Additional components, Docker, AppImage, Ubuntu Snap
- Basics: About FreeCAD, Interface, Mouse navigation, Selection methods, Object name, Preferences, Workbenches, Document structure, Properties, Help FreeCAD, Donate
- Help: Tutorials, Video tutorials
- Workbenches: Std Base, Assembly, BIM, CAM, Draft, FEM, Inspection, Mesh, OpenSCAD, Part, PartDesign, Points, Reverse Engineering, Robot, Sketcher, Spreadsheet, Surface, TechDraw, Test Framework
- Hubs: User hub, Power users hub, Developer hub