Draft Facebinder
Draft Facebinder |
Menu location |
---|
Draft → Facebinder |
Workbenches |
Draft, Arch |
Default shortcut |
F F |
Introduced in version |
0.14 |
See also |
Part Box, Arch Wall |
Description
The Facebinder tool creates a surface object from the selected faces of a solid object. It is parametric, meaning that if you modify the original object, the Facebinder updates accordingly. If you move and rotate the Facebinder, it will stay linked to the original faces.
It can be used to create an extrusion from a collection of faces from other objects. A typical use is in architectural design to build an object that covers several walls, for example, a wall paper, or wall finish.
Facebinder created from the faces of solid walls
Usage
- Pick one face, or hold Ctrl and pick several faces, from solid objects.
- Press the Facebinder button, or press F then F keys.
The Facebinder can be edited by double clicking on the element in the tree view. Then you can change the faces that are part of the object.
- To add a face, click on a face of a solid object in the 3D view, and then click on the Add button.
- To remove a face, select one of the sub-elements in the list, and then click on the Remove button.
- Press Esc or the OK button to complete the edition.
Options
This object has no options when it's being created. Only selected faces will be used to create the Facebinder object.
Properties
Data
- DataExtrusion: specifies an extrusion thickness to apply to all faces of the shape.
- DataRemove Splitter: if it is
true
it tries to fuse the internal intersections of the Facebinder when it extruded. - DataSew: if it is
true
it tries to perform a topological sewing operation on the Facebinder when it extruded. - DataOffset: specifies an offset distance to apply betweenthe facebinder and the original faces, prior to extrusion.
- DataArea: the total area of this facebinder.
View
- ViewPattern: specifies a Draft Pattern with which to fill the face of the shape. This property only works if ViewDisplay Mode is "Flat Lines".
- ViewPattern Size: specifies the size of the Draft Pattern.
Scripting
See also: Draft API and FreeCAD Scripting Basics.
The Facebinder tool can be used in macros and from the Python console by using the following function:
Facebinder = makeFacebinder(selectionset)
- Creates a
Facebinder
object from the givenselectionset
, which is a list ofSelectionObject
s as returned byFreeCADGui.Selection.getSelectionEx()
. Only selected faces are taken into account.selectionset
can also be aPropertyLinkSubList
.
A PropertyLinkSubList
is a list of tuples; each tuple contains as first element an object
, and as second element a list (or tuple) of strings; these strings indicate the names of the sub-elements (faces) of that object.
PropertyLinkSubList = [tuple1, tuple2, tuple3, ...]
PropertyLinkSubList = [(object1, list1), (object2, list2), (object3, list3), ...]
PropertyLinkSubList = [(object1, ['Face1', 'Face4', 'Face6']), ...]
PropertyLinkSubList = [(object1, ('Face1', 'Face4', 'Face6')), ...]
The thickness of the Facebinder can be added by overwriting its Extrusion
attribute; the value is entered in millimeters.
The placement of the Facebinder can be changed by overwriting its Placement
attribute, or by individually overwriting its Placement.Base
and Placement.Rotation
attributes.
Example:
import FreeCAD
import FreeCADGui
import Draft
# Insert a solid box
Box = FreeCAD.ActiveDocument.addObject("Part::Box", "Box")
Box.Length = 2300
Box.Width = 800
Box.Height = 1000
# selection = FreeCADGui.Selection.getSelectionEx()
selection = [(Box, ("Face1", "Face6"))]
Facebinder = Draft.makeFacebinder(selection)
Facebinder.Extrusion = 50
FreeCAD.ActiveDocument.recompute()
Facebinder.Placement.Base = FreeCAD.Vector(1000, -1000, 100)
Facebinder.ViewObject.ShapeColor = (0.99, 0.99, 0.4)
- 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, Material, Mesh, OpenSCAD, Part, PartDesign, Points, Reverse Engineering, Robot, Sketcher, Spreadsheet, Surface, TechDraw, Test Framework
- Hubs: User hub, Power users hub, Developer hub