Draft PathArray
Yol dizisi |
Menü konumu |
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Draft → PathArray |
Tezgahlar |
Draft, Arch |
Varsayılan kısayol |
Hiçbiri |
Versiyonda tanıtıldı |
- |
Ayrıca bkz |
Draft Array |
Description
The Draft PathArray tool places copies of a selected shape along a selected path, which can be a Draft Wire, a Draft BSpline, and similar edges.
The PathArray tool can be used on any object that has a Part TopoShape, meaning 2D shapes created with the Draft Workbench, but also 3D solids created with other workbenches, for example, Part, PartDesign, or Arch.
- To create orthogonal, polar or circular arrays, use the corresponding OrthoArray, PolarArray, or CircularArray tools.
- To position App Link copies along a path use PathLinkArray.
- To position copies at specified points use PointArray.
- To create copies and manually place them use Move or Rotate.
- To create exact copies and manually place or scale them, use Clone or Std LinkMake.
Object arranged along a path
Usage
- Select the object that you wish to distribute.
- Select the path object or edges along which the object will be distributed.
- Press the PathArray button.
- The Array object is immediately created. You must change the properties of the array to change the number and direction of copies created.
Each element in the array is an exact clone of the original object, but the entire array is considered a single unit in terms of properties and appearance.
Note: if the VeriBase object doesn't seem to be positioned correctly in the path, check that its VeriPlacement is in the origin (0,0,0)
. Certain objects can be placed anywhere in the 3D space when used with the PathArray tool, but others must be at the origin, particularly those created by using Part Extrude with a 2D profile like a Sketch.
Options
There are no options for this tool. Either it works with the selected objects or not.
Properties
A PathArray is derived from a Part Feature (Part::Feature
class), therefore it shares all the latter's properties. In addition to the properties described in Part Feature, the PathArray has the following properties in the property editor.
Alignment
- VeriAlign (
Bool
): if it istrue
the copies will be aligned to the path; otherwise they are left in their default orientation.
- Note: in certain cases the shape will appear flat, in reality it may have moved in the 3D space, so instead of using a flat view, change the view to axonometric.
- VeriAlign Mode (
Enumeration
): three modes,Original
,Frenet
,Tangent
. - VeriExtra Translation (
VectorDistance
): additional displacement vector(x, y, z)
that will be applied to each copy along the path. This is useful to make small adjustments in the position of the copies, for example, when its reference point doesn't match the center point of its shape. - VeriForce Vertical (
Bool
): if it istrue
, the value of VeriVertical Vector will be used as the local Z direction, when VeriAlign Mode isOriginal
orTangent
. introduced in version 0.19 - VeriTangent Vector (
Vector
): it defaults to(1, 0, 0)
; alignment unit vector that will be used when VeriAlign Mode isTangent
. introduced in version 0.19 - VeriVertical Vector (
Vector
): it defaults to(0, 0, 1)
; unit vector of the local Z direction that will be used when VeriVertical Vector istrue
. introduced in version 0.19
Objects
- VeriBase (
LinkGlobal
): specifies the object to duplicate in the path. - VeriCount (
Integer
): specifies the number of copies to create in the path. - VeriPath Object (
LinkGlobal
): specifies the object along which the copies will be distributed. It must contain'Edges'
in its Part TopoShape; for example, it could be a Wire or BSpline. - VeriPath Subelements (
LinkSubListGlobal
): specifies the sub-elements (edges) of the VeriPath Object on which the copies will be created. The copies will be created only on these edges. If this property is empty, the copies will be distributed on the entire VeriPath Object.
Scripting
See also: Draft API and FreeCAD Scripting Basics.
The PathArray tool can be used in macros and from the Python console by using the following function:
Older call
path_array = makePathArray(base_object, path_object, count, xlate=None, align=False, pathobjsubs=[])
New call
path_array = make_path_array(base_object, path_object,
count=4, extra=App.Vector(0, 0, 0), subelements=None,
align=False, align_mode="Original", tan_vector=App.Vector(1, 0, 0),
force_vertical=False, vertical_vector=App.Vector(0, 0, 1),
use_link=True):
- Creates a
"PathArray"
object from thebase_object
, by placing as many ascount
copies alongpath_object
.- If
extra
is given, it is a vector that displaces each of the individual copies by a small amount. - If
subelements
is given, it is a list of edges ofpath_object
, for example,['Edge1', 'Edge2']
; the copies will be created along this shorter path. - If
align
isTrue
, the copies are aligned along thepath_object
depending on the value ofalign_mode
, which may be"Original"
,"Frenet"
or"Tangent"
. - If
tan_vector
is given, it is a unit vector that defines the local tangent direction of the copy along the path. It is used whenalign_mode
is"Tangent"
. - If
force_vertical
isTrue
, the value ofvertical_vector
is used to determine the local Z direction of the copy along the path. It is used whenalign_mode
is"Original"
or"Tangent"
. - If
use_link
isTrue
, the type of array created will be a PathLinkArray, whose elements are App Link instances instead of simple copies.
- If
Example:
import FreeCAD as App
import Draft
doc = App.newDocument()
p1 = App.Vector(500, -1000, 0)
p2 = App.Vector(1500, 1000, 0)
p3 = App.Vector(3000, 500, 0)
p4 = App.Vector(4500, 100, 0)
spline = Draft.make_bspline([p1, p2, p3, p4])
obj = Draft.make_polygon(3, 500)
path_array = Draft.make_path_array(obj, spline, 6)
doc.recompute()
wire = Draft.make_wire([p1, -p2, -p3, -p4])
path_array2 = Draft.make_path_array(obj, wire, count=3, extra=App.Vector(0, -500, 0), subelements=["Edge2", "Edge3"], align=True, force_vertical=True)
doc.recompute()
Technical explanation for the Align property
When VeriAlign is false
, the placement of the copied shapes is easy to understand; they are just moved to a different position in their original orientation.
Object arranged along a closed path in the original orientation
When VeriAlign is true
, the positioning of the shapes becomes a bit more complex:
- First, Frenet coordinate systems are built on the path: X is tangent, Z is normal, Y is binormal.
- Then the original object is copied to every on-path coordinate system, so that the global origin is matched with the on-path coordinate system origin.
Object arranged along a closed path; description of components and path
The following images show how the array is produced, depending on which plane the path is.
Path on XY Plane:
Object arranged along a closed path which is aligned to the XY plane
Path on XZ Plane:
Object arranged along a closed path which is aligned to the XZ plane
Path on YZ Plane:
Object arranged along a closed path which is aligned to the YZ plane
As you reorient the path but not the object, the result is consistent: the object remains aligned to the path the way it was before reorienting the path.
Editor: thank you to user DeepSOIC for this explanation.
Additional alignment modes and options introduced in v0.19
Original mode (the default) is the historic alignment mode as in version 0.18. It is not really the Frenet alignment. Original mode uses the normal parameter from Draft.getNormal (or the default) as a constant - it does not calculate curve normal. X follows the curve tangent, Y is the normal parameter, Z is X.Cross(Y).
Tangent mode is similar to Original, but includes a rotation to align the Base object's X to the TangentVector before placing copies. After the rotation, Tangent behaves the same as Original. In previous versions this rotation would be performed manually before invoking PathArray.
Frenet mode orients the copies to a coordinate system along the path. X is tangent to curve, Y is curve normal, Z is curve binormal. If a normal can not be computed (ex a straight line), the default is used.
The ForceVertical option applies to Original and Tangent modes. When this option is applied, the normal parameter from Draft.getNormal is ignored. X follows the curve tangent, Z is the VerticalVector property and Y is X.Cross(Z).
Version 18 cycle chain - Original mode
Railway cross ties (sleepers) - Tangent mode + ForceVertical
Frenet Mode
- 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