Help for Rhino Assembly 1.0Rhino Assembly Tutorials
For a quick guide to Rhino Assembly, please go to our tutorials page.
Rhino Assembly Overview
With Rhino Assembly plug-in you can position your rigid 3D parts with respect to each other by specifying assembly constraints (fixation, concentricity, coincidence, parallelism, perpendicularity, or tangency) and driving dimensions (distance and angle) between their faces and edges.
Assembly plugin automatically satisfies all constraints and dimensions making a consistent assembly from existing parts. An assembled mechanism can then be animated by varying a parameter of one or several of its driving dimensions. The Assembly Manager panel allows navigation over all assembly constraints and driving dimensions imposed on geometric elements of a designed model.
Assembly Toolbar
You may access the tools offered by the Rhino Assembly from either the Assembly Toolbar or
by typing the corresponding commands in the "Command:" line.
Creating Assembly Constraints and Driving Dimensions
Assembly constraints and driving dimensions are imposed on previously created 3D parts.
Existing edges and faces of polysurfaces can be used to set the constraints and
driving dimensions. To set a constraint in your model, give a command that corresponds to the desired constraint type or click corresponding icon on the Assembly Toolbar and
then select the edges or surfaces by clicking them in the Rhino working area.
It is also possible to create a constraint by selecting geometrical objects prior to
calling the constraint creation command. In this case constraint is created for the selected objects.
 Constraints between objects belonging to the same polysurface are not allowed.
Supported types of geometric elements are:
-
Canonic edges of a polysurface: straight edges and circular arcs
-
Canonic faces of a polysurface: faces of planar, cylindrical or spherical geometry (including trimmed faces)
-
Isolated objects: single points, straight segments and circular arcs (not included into a polyline)
Available constraint types are:
- 1. Concentricity
Toolbar button:  Rhino command: LDDConcentricity
Supported argument types: Point, Circle, Cylinder, Sphere
Concentricity also implies coaxiality, where applicable (for example, for a pair of cylinders)
- 2. Coincidence
Toolbar button:  Rhino command: LDDCoincidence
Supported argument types:
| Coincidence | Point | Line | Circle | Plane | Cylinder | Sphere |
| Point | x | x | x | x | x | x |
| Line | x | x | | x | x | |
| Circle | x | | x | x | x | x |
| Plane | x | x | x | x | | |
| Cylinder | x | x | x | | x | |
| Sphere | x | | x | | | x |
- 3. Parallelism
Toolbar button:  Rhino command: LDDParallelism
Supported argument types: Line, Plane, Circle, Cylinder
- 4. Perpendicularity
Toolbar button:  Rhino command: LDDPerpendicularity
Supported argument types: Line, Plane, Circle, Cylinder
- 5. Tangency
Toolbar button:  Rhino command: LDDTangency
Supported argument types: Line, Plane, Circle, Cylinder, Sphere
- 6. Distance
Toolbar button:  Rhino command: LDDDistance
Supported argument types: Point, Line, Plane, Circle, Cylinder, Sphere
For a sphere distance is measured from its center, for a cylinder distance is measured from its axis.
- 7. Angle
Toolbar button:  Rhino command: LDDAngle
Supported argument types: Line, Plane, Circle, Cylinder
For directional constraints like Angle, Parallelism and Perpendicularity angle is measured in 3D between directions of the objects from 0 to 180 degrees. Direction of a cylindrical surface is the direction of its axis. Direction of a circle is the direction of the normal vector of its plane. Planar surfaces are
handled in a different way: angle is measured between directed object and the plane itself (not its normal).
Upon creation of a dimension (Angle or Distance) the plug-in computes a
default value for its parameter after the dimension arguments are selected. This value
is taken from the current geometrical position of the selected objects and it is
printed in the command prompt. To use this value for newly created dimension just
hit Enter when asked about a value. This value can be changed later
via Constraint Properties panel.
Sometimes default value can't be computed, e.g. when a Distance dimension is created
for intersecting planes.
The constraint or dimension you created will be added to the list model constraints, but it is not
displayed in the working area — to manage the existing constraints, you should use the Assembly Manager panel. By default newly created constraints
are applied immediately – Rhino Assembly moves the geometrical objects to satisfy all constraints and dimensions.
Angle Dimension with Axis (Planar Angle)
Upon creation of Angle dimension for a pair of directed objects it is possible to
specify third directed object which is considered as an axis of angle measurement. This third object is
automatically constrained to be perpendicular both to the first and the second objects. To specify an
axis one should press C key after selection of a pair of directed objects while creating
the angle dimension. A planar face can also be used for axis specification; normal vector of
the plane is considered as an axis in this case.
When axis is specified the parameter of angle dimension can take
any value, however two parameters which differ by 360 degrees correspond to the same angle. Using
of axis specification allows to animate several revolutions of a rotated part, to obtain two
revolutions just specify 0 and 720 as start and end animation parameters for the angle dimension.
Fixating Objects
Toolbar button: 
Rhino command: LDDFixation
Allows you to fixate an object. After applying this command, select the entities you are going to fixate and hit Enter.
Fixation prevents an object from moving during computations performed by Rhino Assembly, but it
doesn't prevent it from being moved by user. The fixation can be applied to a whole polysurface as well
as to its part or a single object. When you fix a planar face of a polysurface the polysurface may slide
along the plane (or rotate if you fix a cylindrical face).
Creation of Rigid Sets
Toolbar button: 
Rhino command: LDDRigidSet
Allows you to create a Rigid Set containing several geometrical objects. Creation of a
rigid set fixates several objects together. After applying this command, select the entities you are
going to fixate together and hit Enter.
An object can't be put into several different rigid sets.
Entire polysurface can be put into a rigid set, while sub-surfaces can not.
Objects contained in the same Rigid Set can be moved or rotated only all together;
Rhino Assembly can not change their mutual positions. However their mutual position can be changed by
user (by dragging the objects for example).
Assembly Manager
Toolbar button: 
Rhino command: LDDManager
 Displays the Assembly Manager panel. Assembly Manager allows you to view, edit or delete the constraints you created
and to manage the animation of the dimensions.
When you select a constraint in the Assembly Manager the objects linked with this
constraint are highlighted in the Rhino working area. Conversely, if some geometry is selected
constrains related to it become bold in the Assembly Manager.
Update Automatically check-box which defines
how the model is updated. Color indicator near this check-box can be green,
yellow or red depending on the status of the constraints and dimensions
(see Updating Geometry section for details).
Assembly Manager supports selection of multiple constraints. Several constraints can be
selected as usual with use of the Shift or Ctrl keys, then user can animate
the selected dimensions all together or remove them from the model by hitting the Delete
key or clicking Delete in the context menu.
Assembly Manager is dockable you can fix it near any side of Rhino window simply by dragging
it to a desired place.
Editing Constraints and Driving Dimensions Properties
Open the Assembly Manager window, select the constraint you are going to edit.
Double click it or click right mouse button and select "Edit..." from the context menu. The Constraint Properties panel will open, where you can modify the constraint name and/or dimension value. Also, you can change there animation parameters for the selected dimension (angle or distance). Turn off Enabled check-box in order to temporary disable particular constraint or driving dimension.
Clicking any of the ruler buttons 
allows you to automatically insert a value computed from
the current positions of your objects into the corresponding field of the Constraint Properties
panel. Arrow-buttons allow user to increment or decrement values stored
in the fields for driving dimensions.
If Update Automatically check-box on the Assembly Manager panel is turned on
a modification of the driving dimension value with help of arrow-buttons
results in the recalculation of the positions of model objects.
Clicking the Flip Side button changes mutual position of the constrained objects.
For example if a plane is tangent to a cylinder, clicking this button for the Tangency constraint
will move the cylinder to the another side of the plane.
Constraint Properties panel is dockable you can fix it near any side of Rhino window
simply by dragging it to a desired place.
Updating Geometry
Rhino Assembly supports two different modes for updating the model. The first mode is
the automatic one (default). The second mode is the manual updating. Switching
between the modes is done via the Update Automatically check-box on the Assembly
Manager panel.
Automatic Update
In the automatic mode constraints and dimensions are applied to the parts of your assembly
immediately. Updating of the model occurs automatically after the following events
- constraint or dimension is created/deleted
- parameter of a driving dimension is changed
- geometrical object is moved, rotated or dragged by user
After any of these actions Rhino Assembly recalculates the model and moves the objects
to satisfy the constraints and dimensions.
Manual Update
Toolbar button: 
Rhino command: LDDUpdate
When the Update Automatically check-box is disabled Rhino Assembly recalculates
the positions of the objects only when user explicitly asks to do that.
If some of constraints or driving dimensions cannot be satisfied, the error message will appear.
Status Indicator
Thе colors of the status indicator near the Update Automatically check-box have
the following meaning
-
 - all constraints and dimensions are satisfied. Appears in the case of successful recalculation.
-
 - the status of constraints in the model is unknown. In the
automatic updating mode it appears when the model is modified by a Rhino command which
is not a moving, rotating or dragging, also it appears when the model
is just opened from a .3dm file. When the automatic updating is turned off this indicator
appears after any modification of the geometry or constraints. To update the state of the model
call LDDUpdate command or click
icon or double-click the indicator itself.
-
 - some of the constraints or driving dimensions are violated.
Appears when there is a contradiction between constraints or parameters
of driving dimensions and all constraints can't be satisfied. In this case remove
contradictory constraints or correct the parameters in order to make the model consistent.
Animation
Rhino Assembly provides a possibility to animate the model by varying the parameter of a single
or multiple driving dimensions
Single Dimension Animation
Open the Assembly Manager window, and right-click on the dimension (angle or distance) you are going to animate. Select "Animate..." from the context menu,
or press "Animate..." button on the Constraint Properties panel.
The Animation control panel will open and plug-in will start to compute animation frames in background according to the current animation settings for this constraint.
User can change the animation
parameters by editing them in the Constraint Properties panel.
Animation starts from the value of the dimension parameter specified in the Start Value
field and the parameter is incremented up to (decremented down to) the value from the End Value
field. The number of frames specified in the Frames field defines how smooth the animation is.
The Time field is used to specify the time taken by the entire animation, specify zero value
to obtain the fastest animation (time will depend only on the performance of your system).
These parameters are stored in .3dm file.
Animating Multiple Dimensions
In order to animate the assembly by varying the parameters of several driving dimensions
open the Constraint Properties panel and specify Start and End Values for each dimension you're
going to animate (in the same way as it is done for single dimension animation).
Then select these dimensions in the Assembly Manager holding Shift or Ctrl keys.
Constraint Properties panel will be changed, it will have only Frames and Time
fields where you can specify needed values. To start the animation hit the Animate button on
the Constraint Properties panel.
Animating All the Dimensions
Toolbar button: 
Rhino command: LDDAnimate
When this command is called all the dimensions are animated according to the parameters
specified for them on the Constraint Properties panel.
Animation Control Panel (Player)
When single or multiple dimensions are animated Animation Control Panel is opened. It
allows you to control animation process and navigate through the frames. This panel is opened
right after the user clicks the "Animate" button.
The roles of the buttons are quite traditional
 – starts playing the animation, direction of playing depends on where you’ve clicked the button,
 – stops the animation at the current frame (available only while playing),
 – click once to move the animation one frame backward (forward), hold the mouse button to scroll the animation backward (forward),
– click to set the animation to the beginning (to the end).
You can also drag the slider with a mouse to navigate though animation frames. Check-box
Backward makes animation to be replayed backward after the end is reached.
Check-box Repeat makes animation to be played continuously until the
Pause button is hit.
You can also specify the time taken by the animation in the
Time box, specify zero value to obtain the fastest animation (time will depend
only on the performance of your system).
Use «Edit...» button in order to modify number of frames in the animation,
start and end values of the constraint's parameter, it is done via Constraint Properties panel.
Press Apply button if you want to
use the current frame as a new state of your model. Hit Cancel if you want to return to
the state before the animation.
Help and About Box
Toolbar button: 
Rhino command: LDDAbout
Opens About Box for Rhino Assembly plug-in. Click there
Help Page link to open this manual in your browser. Or if you have purchased
the product and have a license key click "Register..." button in order to
unlock the functionality locked in the evaluation version.
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