|Draft → Facebinder|
|Introduced in version|
|Part Box, Arch Wall|
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
- Pick one face, or hold and pick several faces, from solid objects.
- Press the button, or press then 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 button.
- To remove a face, select one of the sub-elements in the list, and then click on the button.
- Press or the button to complete the edition.
This object has no options when it's being created. Only selected faces will be used to create the Facebinder object.
- DataExtrusion: specifies an extrusion thickness to apply to all faces of the shape.
- DataRemove Splitter: if it is it tries to fuse the internal intersections of the Facebinder when it extruded.
- DataSew: if it is it tries to perform a topological sewing operation on the Facebinder when it extruded.
- 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.
Facebinder = makeFacebinder(selectionset)
- Creates a
Facebinderobject from the given
selectionset, which is a list of
SelectionObjects as returned by
FreeCADGui.Selection.getSelectionEx(). Only selected faces are taken into account.
selectionsetcan also be 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
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)