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
See also: Property editor.
A Draft Shape2DView object is derived from a Part Part2DObject and inherits all its properties. It also has the following additional properties:
Data
Draft
- DataBase (
Link
): specifies the object to be projected. - DataFace Numbers (
IntegerList
): specifies the indices of the faces to be projected. Only works if DataProjection Mode isIndividual Faces
. - DataFuse Arch (
Bool
): specifies if Arch objects of the same type and material are fused or not. - DataHidden Lines (
Bool
): specifies if hidden lines are shown or not. - DataIn Place (
Bool
): only works if the selected object is an Arch SectionPlane, and DataProjection Mode isCutlines
orCutfaces
, specifies if the resulting projection will appear co-planar with the section plane. - DataProjection (
Vector
): specifies the direction of the projection. - DataProjection Mode (
Enumeration
): specifies the projection mode. The following modes are available:Solid
: projects the entire selected object.Individual Faces
: only projects the faces in the DataFace Numbers list.Cutlines
: only works if the selected object is an Arch SectionPlane, projects only the edges cut by the section plane.Cutfaces
: only works if the selected object is an Arch SectionPlane, projects the areas cut through solids by the section plane as faces.Solid faces
: projects the entire selected object by cutting faces one by one. Can be used if theSolid
mode gives wrong results. introduced in version 0.20
- DataSegment Length (
Float
): specifies the size in millimeters of linear segments if DataTessellation istrue
. - DataTessellation (
Bool
): specifies if tessellation should be performed. Tessellation means that curves are replaced by sequences of line segments. This can be computationally intensive if the DataSegment Length is too short. - DataVisible Only (
Bool
): specifies if the projection should only be recomputed if it is visible.
View
Draft
- ViewPattern (
Enumeration
): not used. - ViewPattern Size (
Float
): not used.
Scripting
See also: Autogenerated API documentation and FreeCAD Scripting Basics.
To create a 2D projection use the make_shape2dview
method (introduced in version 0.19) of the Draft module. This method replaces the deprecated makeShape2DView
method.
shape2dview = make_shape2dview(baseobj, projectionVector=None, facenumbers=[])
baseobj
is the object to be projected.projectionVector
is the projection vector. If not supplied the Z axis is used.facenumbers
is a list of face numbers (0-based). If supplied only these faces are considered.shape2dview
is returned with the created 2D projection.
Change the ProjectionMode
property of the created object if required. It can be: "Solid"
, "Individual Faces"
, "Cutlines"
, "Cutfaces"
or "Solid faces"
.
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