Placement is how FreeCAD specifies the location and attitude (orientation) of an object in space. Placement can be specified in multiple forms and manipulated via scripting, the Properties pane or the Placement dialog (Edit menu).
Accessing the Placement Attribute
An object's Placement attributes can be accessed and modified in 3 ways:
Forms of Placement
The placement is stored internally as a position, and a rotation (rotation axis and angle transformed into a quaternion ). While there are several forms to specify a rotation, for instance with a rotation center, this is only used to affect the rotation computation and is not stored for later operations. Similarly, if a rotation axis of (1,1,1) is specified, it may be normalized when stored in the quaternion and appear as (0.58, 0.58, 0.58) when browsing the object later.
Angle, Axis and Position
Placement = [Angle, Axis, Position]
The first form of Placement fixes an object's location in space with a Position, and describes its orientation as a single rotation about an axis.
Angle = r is a scalar indicating the amount of rotation of the object about Axis. Entered as degrees, but stored internally as radians.
Axis = (ax,ay,az) is a vector describing an axis of rotation (See Note about axis of rotation). Examples are:
(1,0,0) ==> about X axis (0,1,0) ==> about Y axis (0,0,1) ==> about Z axis (0.71,0.71,0) ==> about the line y=x
Note that it is also possible to translate (move) an object along this axis of rotation (axial motion) by entering the distance to move in the Axial spinbox and clicking the Apply axial button. (One way to envision axial motion is to think of an airplane with a propeller spinning on its nose -- the propeller spins about an axis of rotation while the plane moves along that same axis.) The values in the vector can be thought of as the relative amount of motion that will be applied in that direction. For example, in the y=x case (0.71,0.71,0) the value contained in the Axial spinbox gets applied in equal measure to the X and Y directions, but no movement happens in the Z direction.
Position = (x,y,z) is a Vector describing the point from which the object's geometry will be calculated (in effect, a "local origin" for the object). Note that in scripts, Placement.Base is used to denote the Position component of a placement. The Property Editor calls this value "Position" and the Placement dialog calls it "Translation".
Position and Yaw, Pitch and Roll
Placement = [Position, Yaw-Pitch-Roll]
The second form of Placement fixes an object's location in space with a Position (as in the first form), but describes it's orientation using Yaw, Pitch and Roll angles (Yaw, Pitch, Roll). These angles are sometimes referred to as Euler angles or Tait-Bryan angles (Euler angles). Yaw, Pitch and Roll are common aviation terms for a body's orientation (or attitude).
Position = (x,y,z) is a Vector describing the point from which the object's geometry will be calculated (in effect, a "local origin" for the object).
Yaw-Pitch-Roll = (y,p,r) is a tuple that specifies the attitude of the object. Values for y,p,r specify degrees of rotation about each of the z,y,x axis (see note).
>>> App.getDocument("Sans_nom").Cylinder.Placement=App.Placement(App.Vector(0,0,0), App.Rotation(10,20,30), App.Vector(0,0,0))
App.Rotation(10,20,30) = Euler Angle
Yaw = 10 degrees (Z)
Pitch = 20 degrees (Y)
Roll = 30 degrees (X)
Yaw is the rotation about the Z axis, that is to say a rotation from left to right.
(The yaw angle is the Psi ψ).
Pitch is rotation about the Y axis, that is to say nose-up and nose-down.
(The Pitch angle is the Phi φ).
Roll is rotation about the X axis, that is to say wing up and down.
(The Roll angle is the Thêta θ).
Placement = Matrix
The third form of Placement describes the object's position and orientation with a 4x4 affine transformation matrix (Affine Transformation).
((r11,r12,r13,t1), (r21,r22,r23,t2), (r31,r32,r33,t3), (0,0,0,1)) , with rij specifying rotation and ti specifying translation.
The Placement Dialog
The Placement Dialog is invoked from the Edit menu. It is used to precisely rotate/translate objects. It is also used when we need to create a sketch on a "non standard" plane or change a sketch's orientation to a new plane.
The Translation section adjusts the object's location in space. The Center section adjusts the rotational axis to one that does not pass through the object's reference point. The Rotation section adjusts the rotational angle(s) and the method of specifying those angles.
But while the elements within each section generally apply to the purpose of that section there are also some elements in one section that can affect elements in another section. For example, clicking the Selected points button in the Center section with 2 points selected in the 3d view results in not only populating the Center coordinate spinboxes with the coordinates of the midpoint between those 2 selected points, but it also creates a custom axis along the line defined by those 2 selected points in the Rotation section. In another example, placing a value in the Axial spinbox and clicking the Apply axial button in the Translation section translates (moves) the object along the axis defined in the Rotation section.
The Apply incremental changes to object placement tick box is useful when translations/rotations are to be made relative the object's current position/attitude, rather than to the original position/attitude. Ticking this box resets the dialogue input fields to zero, but does not change the object's orientation or location. Subsequent entries do change the orientation/location, but are applied from the object's current position. Enabling this checkbox is also useful when using the Selected points button as it can sometimes prevent undesired placement changes.
PS: since version 0.17 introduce new object Part, this object have his placement, and the Placement object created in the Part object is incremented with the Part Placement. introduced in version 0.17 For obtain the Part Placement use this code
import Draft, Part sel = FreeCADGui.Selection.getSelection() print sel.Placement print sel.getGlobalPlacement() # return the GlobalPlacement print sel.getParentGeoFeatureGroup() # return the GeoFeatureGroup, ex: Body or a Part. print "____________________"
Selected points button is used to populate the coordinates in the Center coordinates spinboxes and (when 2 or 3 points are selected) additionally to create a custom (user-defined) axis of rotation in the Rotation section. A point can be a vertex, but it can also be any point along an edge or on a face. When you select an edge or face the entire edge or face is selected, but FreeCAD also remembers which point on that face or edge the mouse pointer was hovering over when that edge or face was selected. It is this point's coordinates that get used in the Placement dialog when the Selected points button is clicked. You might be thinking this isn't a very precise way of selecting a point, and you are correct, but in many cases it is sufficient that the point selected is guaranteed to be on that edge or face. In cases where you need to precisely designate a point to be used you should select a vertex. When there is no vertex in the desired location consider creating one, perhaps in a temporary sketch attached to that face or edge, perhaps using a Draft workbench object, such as a line or point, etc.
Let us first consider the simple case of selecting 1 point. The workflow is to first select the desired point, then click the Selected points button. The coordinates of the selected point will be used to populate the X, Y, and Z spinboxes within the Center section. Now any rotation done on the object will about this center of rotation.
Now consider the case of selecting 2 points. You would select the 2 desired points, and then click the Selected points button. The coordinates of the midpoint between the 2 selected points get placed into the X, Y, and Z spinboxes within the Center section. Now any rotation done on the object will be about this center of rotation. But in addition to setting up the Center section coordinates a custom (user-defined) axis is also added to the Axis element within the Rotation section. (Note: if you were in Euler rotation mode, the mode gets switched to Rotation with an axis mode and the new custom axis is selected as the current axis of rotation.) Now any rotation done using the new custom axis will be about this axis of rotation. As an added bonus, the distance is measured between the 2 selected points, and this information is given in the Report View. (Note: Hold down the Shift key while clicking the Selected points button to copy the distance measurement to the clipboard.) By entering this distance into the Axial spinbox in the Translation section and clicking the Apply axial button you can translate (move) the object so that the first selected point now occupies the coordinates occupied by the second selected point (at the time the Selected points button was clicked).
Now consider the case of selecting 3 points. You would select the 3 desired points, and then click the Selected points button. The coordinates of the first selected point (order of selection is very important here) get placed into the X, Y, and Z spinboxes within the Center section. Since 3 points define a plane FreeCAD is able to take advantage of that and use those 3 points to create a new custom (user-defined) axis of rotation that is normal (perpendicular) to that defined plane. As with 2 selected points, the distance between points is also shown in the Report View, but this time it is the distance between the 2nd and 3rd selected points. (Note: Hold down the Shift key while clicking Selected points button -- Shift + Click -- to copy the angle measurement to the clipboard.) Additionally, the angle between the 2nd and 3rd points is also measured and displayed in the Report View. By entering this angle into the Angle spinbox within the Rotation section we can very precisely rotate the object such that now the 2nd selected point is in alignment with the coordinates occupied by the 3rd selected point. (Note: you might want to increase the number of digits used within the Edit menu -> Preferences -> General -> Units -> Number of decimals spinbox if you desire more precision.)
Rotations about a single axis:
Before Rotation (top view)
After Rotation about Z (top view)
After Rotation about y=x (right view)
Rotation with offset centre point:
Before Rotation (top view)
After Rotation about Z (top view)
Rotation using Euler angles:
Placement.Base vs Shape Definition
Placement is not the only way to position a shape in space. Note the Python console in this image:
Both cubes have the same value for Placement, but are in different locations! This is because the 2 shapes are defined by different vertices (curves in more complex shapes). For the 2 shapes in the above illustration:
>>> ev = App.ActiveDocument.Extrude.Shape.Vertexes >>> for v in ev: print v.X,",",v.Y,",",v.Z ... 30.0,30.0,0.0 30.0,30.0,10.0 40.0,30.0,0.0 40.0,30.0,10.0 40.0,40.0,0.0 40.0,40.0,10.0 30.0,40.0,0.0 30.0,40.0,10.0 >>> e1v = App.ActiveDocument.Extrude001.Shape.Vertexes >>> for v in e1v: print v.X,",",v.Y,",",v.Z ... 0.0,10.0,0.0 0.0,10.0,10.0 10.0,10.0,0.0 10.0,10.0,10.0 10.0,0.0,0.0 10.0,0.0,10.0 0.0,0.0,0.0 0.0,0.0,10.0 >>>
The Vertices (or Vectors) that define the shape use the Placement.Base attribute as their origin. So if you want to move a shape 10 units along the X axis, you could add 10 to the X coordinates of all the Vertices or you could set Placement.Base to (10,0,0).
Using "Center" to Control Axis of Rotation
By default, the axis of rotation isn't really the x/y/z axis. It is a line parallel to the selected axis, but passing through the reference point (Placement.Base) of the object to be rotated. This can be changed by using the Center fields in the Placement dialog or, in scripts, by using the Center parameter of the FreeCAD.Placement constructor.
For example, suppose we have a box (below) positioned at (20,20,10).
We wish to spin the box around it's own vertical centre line (ie local Z), while keeping it the same position. We can easily achieve this by specifying a Center value equal to the coordinates of the box's central point (25,25,15).
In a script, we would do:
import FreeCAD obj = App.ActiveDocument.Box # our box rot = FreeCAD.Rotation(FreeCAD.Vector(0,0,1),45) # 45° about Z #rot = FreeCAD.Rotation(FreeCAD.Vector(1,0,1),45) # 45° about X and 45° about Z #rot = FreeCAD.Rotation(10,20,30) # here example with Euler angle Yaw = 10 degrees (Z), Pitch = 20 degrees (Y), Roll = 30 degrees (X) centre = FreeCAD.Vector(25,25,15) # central point of box pos = obj.Placement.Base # position point of box newplace = FreeCAD.Placement(pos,rot,centre) # make a new Placement object obj.Placement = newplace # spin the box
import FreeCAD obj = App.ActiveDocument.Extrude # our box rot = FreeCAD.Rotation(FreeCAD.Vector(0,0,1),45) # 45 about Z #rot = FreeCAD.Rotation(FreeCAD.Vector(1,0,1),45) # 45° about X and 45° about Z #rot = FreeCAD.Rotation(10,20,30) # here example with Euler angle Yaw = 10 degrees (Z), Pitch = 20 degrees (Y), Roll = 30 degrees (X) centre = FreeCAD.Vector(25,25,0) # "centre" of rotation (where local Z cuts XY) pos = obj.Placement.Base # original placement of obj newplace = FreeCAD.Placement(pos,rot,centre) # make a new Placement object obj.Placement = newplace # spin the box
- Axis and Angle can also be expressed as a quaternion.
- The reference point of an object varies depending on the object. Some examples for common objects:
|Part.Box||left (minx), front (miny), bottom (minz) vertex|
|Part.Sphere||center of the sphere (ie centre of bounding box)|
|Part.Cylinder||center of the bottom face|
|Part.Cone||center of bottom face (or apex if bottom radius is 0)|
|Part.Torus||center of the torus|
|Features derived from Sketches||the Feature inherits the Position of the underlying Sketch. Sketches always start with Position = (0,0,0). This position corresponds to the origin in the sketch.|
- As of version 0.13, update of Placement properties in the Data tab has been disabled for objects created with PartDesign, except for the initial sketch from which the solid will be created. Therefore the Placement of a solid created in PartDesign from a sketch can only be altered by adjusting Placement parameters of the initial construction sketch (the first sketch) from which the solid was created.
- Placement functionality will eventually be handled in the Assembly workbench.