Help for RhinoDirect 0.3
RhinoDirect Overview
RhinoDirect plug-in is an extension of the LEDAS RhinoAssembly for Rhinoceros.
Along with the assembly functionality RhinoDirect plug-in allows you to modify shape of your parts by
adding constraints (fixation, concentricity, coincidence, parallelism, perpendicularity, or tangency) and dimensions (distance and angle) between sub-shapes of the same polysurface.
The figure below shows the plug-in running inside Rhino.
The RhinoDirect plug-in satisfies all constraints and dimensions automatically, and
so makes a consistent model and keeping design intent. You can then modify the model by varying the values of its driving dimensions, such as shortening
distances and changing angles. The RhinoDirect Manager panel allows you to navigate through the list of constraints and driving dimensions.
RhinoDirect Toolbar
You can access the plug-in's tools through the RhinoDirect toolbar or by typing the corresponding commands at
Rhino's command prompt. The toolbar buttons and commands are described below.
Creating Constraints and Driving Dimensions
To create a parametric model, you add constraints and driving dimensions to 3D parts
that already exist in the drawing. The constraints and driving dimensions are
attached to the edges and faces of polysurfaces. To place a constraint, enter the command that
corresponds to the desired type of constraint
(or click the corresponding button on the RhinoDirect toolbar), and then select
the edges or surfaces by clicking on them in Rhino's working area.
Alternatively, it is possible to place constraints by reversing the order of steps: first select the geometric objects, and then enter the constraint command.
In this case, the constraint is applied to the selected objects.
RhinoDirect allows creation of constraints and dimensions between objects belonging to the same polysurface. After updating the model the shape of
polysurface is changed to satisfy the constraints and dimensions. It is possible to place constraints and dimensions for vertices of a polysurface: Rhino does not represent
vertices as separate objects, however RhinoDirect shows you special grip objects for them upon creation of the constraint.
RhinoDirect works with the following types of geometric elements:
-
Vertices of polysurfaces.
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Basic edges of polysurfaces: straight edges and circular arcs.
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Basic faces of polysurfaces: faces of planar, cylindrical, or spherical geometry, including trimmed faces.
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Isolated objects: single points, straight segments, and circular arcs (not including those that are parts of polylines).
RhinoDirect provides the following types of constraints:
- 1. Concentricity
Toolbar button: 
Rhino command: LDDConcentricity
Supported elements: Point, Circle, Cylinder, Sphere
This constraint keeps two elements concentric. Concentricity also implies coaxiality (share the same axis), such as for a pair of cylinders.
- 2. Coincidence
Toolbar button: 
Rhino command: LDDCoincidence
Supported pairs of elements:
| 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 |
This constraint keeps two elements aligned with each other.
- 3. Parallelism
Toolbar button: 
Rhino command: LDDParallelism
Supported elements: Line, Plane, Circle, Cylinder
This constraint keeps two elements parallel to each other.
- 4. Perpendicularity
Toolbar button: 
Rhino command: LDDPerpendicularity
Supported elements: Line, Plane, Circle, Cylinder
This constraint keeps two elements perpendicular to each other.
- 5. Tangency
Toolbar button: 
Rhino command: LDDTangency
Supported elements: Line, Plane, Circle, Cylinder, Sphere
This constraint keeps one element tangent to another.
- 6. Distance
Toolbar button: 
Rhino command: LDDDistance
Supported elements: Point, Line, Plane, Circle, Cylinder, Sphere
This constraint keeps two elements the same distance apart. For spheres,
the distance is measured from their centers; for cylinders and circles,
the distance is measured from their axes (axis of a circle is a
line passing through the center of the circle perpendicular to the circle's plane);
- 7. Radius
Toolbar button: 
Rhino command: LDDRadius
Supported elements: Circle, Cylinder
This constraint modifies radius of a shape.
- 8. Angle
Toolbar button: 
Rhino command: LDDAngle
Supported elements: Line, Plane, Circle, Cylinder
This constraint keeps two elements at a constant angle between each other.
For directional constraints, like Angle, Parallelism
and Perpendicularity, the angle is measured from 0 to 180 degrees
(in 3D between the directions of the objects). The direction of a cylindrical
surface is the direction of its axis. The direction of a
circle is the direction of the normal vector from its plane. Planar surfaces are
handled in a different manner: the angle is measured between the object and the
plane itself, and not its normal.
Upon the creation of a dimension (Distance, Radius or Angle), the plug-in
computes the default value for its parameter after the dimension arguments
are selected. This value is taken from the current geometric position of the
selected objects and it is reported
in the command prompt. To use this value for the newly created dimension, just press
Enter when prompted for the value. The value can be changed later through the
Constraint Properties panel.
Sometimes a default value cannot be computed, such as when a Distance dimension is created for intersecting planes.
By default, newly created constraints are applied immediately to the model;
RhinoDirect moves the geometric objects to satisfy all constraints and dimensions.
The constraints and dimensions are added to the list of model constraints, but they
are not displayed in the working area. To manage constraints, use the
RhinoDirect Manager panel.
Angle Dimension with Axis (Planar Angle)
After placing an Angle dimension between a pair of objects, you can specify a
third object, which is considered the axis of angle measurement. To do so, press
the C key after selecting the first pair of objects. The third object is
constrained automatically to be perpendicular to the first two. You can
also use a planar face for the axis; in this case, the normal vector of
the plane is considered the axis.
If the axis is specified, then the parameter of the angle dimension can take
any value. (Note that when two parameters differ by 360 degrees, they are
at the same angle.) Using the axis allows you to animate several revolutions
of rotated parts. For instance, to rotate the part by two revolutions, specify
0 and 720 as start and ending animation parameters for the angle dimension.
Fixing Objects
Toolbar button: 
Rhino command: LDDFixation
Allows you to fix objects in place. After applying this command, select the
entities you want to fix, and then press Enter. Fixation prevents objects from
moving during computations performed by RhinoDirect, but does not prevent you
from moving them. Fixation can be applied to a whole polysurface, as well as to
part of it, or to a single object. When you fix the planar face of a polysurface,
the polysurface may slide along the plane or may rotate, if you fix a cylindrical
face.
Creating Rigid Sets
Toolbar button: 
Rhino command: LDDRigidSet
Allows you to create a Rigid Set containing several geometric objects.
Creation of a rigid set fixes the objects together. After applying this
command, select the entities you want fixed together, and press Enter.
Entire polysurface can be put into a rigid set as well as its sub-surfaces.
An object cannot be part of more than one rigid set.
Objects contained in the same Rigid Set are moved or rotated together;
RhinoDirect cannot change their relative positions. You can, however, change
their relative positions by dragging the objects apart.
Rigid sets allow you to attach simple geometric objects (e.g. points and lines) to
more complex ones, such as polylines, curves and surfaces. When
RhinoDirect moves a rigid set, it has to satisfy the constraints imposed on
the simple geometry; thus, it also moves all the complex geometry contained in
the same rigid set. This way you can control the position of curves, polylines and
even light sources.
The RhinoDirect Manager
Toolbar button: 
Rhino command: LDDManager
Displays the RhinoDirect Manager panel. RhinoDirect Manager allows you to
view, edit and delete the constraints you created, and
to manage the animation of the dimensions.
When you select a constraint in the RhinoDirect Manager, the objects linked
with the constraint are highlighted in Rhino's working area. Similarly, when you
select geometry in the drawing, the related constraints are shown in boldface in
the RhinoDirect Manager.
The Update Automatically checkbox determines how the model is updated.
The color indicator near the checkbox can be green, yellow, or red depending
on the status of the constraints and dimensions.
(See Updating Geometry section for details).
The RhinoDirect Manager allows you to select several constraints at the same
time using the Shift and Ctrl keys. After you select multiple constraints, you
can then animate them, or else remove them by pressing
the Delete key (or choosing Delete from the context menu).
The RhinoDirect Manager is dockable. You can dock it to any side of the Rhino
window by dragging it to the desired place.
Editing Constraints and Driving Dimensions Properties
To edit the properties of constraints and driving dimensions, follow these steps:
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Open the RhinoDirect Manager window.
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Select the constraint you wish to edit. You can double-click it, or right-click it,
and then select Edit... from the context menu.
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Notice the Constraint Properties panel. Here you can modify the name of the
constraint and the value of the dimension. You can also set the animation parameters
for the selected dimension (distances, radii and angles).
The Enabled checkbox turns the constraint or driving dimension on or off.
Click the ruler buttons 
to automatically insert values computed from the current position of related objects in
the drawing. The values are inserted into the corresponding fields of the Constraint
Properties panel. To increment or decrement values, click the spinner buttons (up and
down arrows next to each value). When the Update Automatically checkbox is
turned on (found on the RhinoDirect Manager panel), changing values
with the spinners recalculates the positions of the objects in
the model.
Clicking the Flip Side button changes relative positions of the constrained objects.
If a plane is tangent to a cylinder, for example, clicking this button moves the
cylinder to the other side of the plane.
The Constraint Properties panel is dockable, so you can dock it to any side of the
Rhino window; simply drag it to the desired place.
Copying and Exporting Objects with Constraints
You can copy and paste a part of your model preserving the constraints imposed on it. To do that just select
the objects you want to copy and press Ctrl+C. After you press Ctrl+V the objects are inserted
into the document and copies of their constraints are inserted into the Constraints Manager. To avoid a
duplication of constraints' names the plug-in adds a numbered postfixes to them.
You can also export a part of a model into a .3dm file keeping the constraints and dimensions. To do that select the
objects you want to export and execute the Export Selected... command from the File menu. Than you can
import this file into another document with File/Import.
Note that if a selected object is linked by constraint with another object which is not selected
this constraint is not copied or exported.
Updating Geometry
RhinoDirect offers two ways to update the model. One is automatic mode, and this is
the default mode. The other mode is manual. You can switch between the two modes
through the Update Automatically checkbox in the RhinoDirect Manager panel.
Automatic Updates
In automatic mode, parts are affected immediately as you apply constraints and dimensions.
The model updates automatically after the following events occur:
- A constraint or dimension is created or deleted.
- A parameter of a driving dimension is changed.
- A geometric object is moved, rotated, or dragged by the user.
After any of these actions occur, RhinoDirect recalculates the model and then
moves the objects (or updates the shapes) to satisfy the constraints and dimensions.
Manual Updates
Toolbar button: 
Rhino command: LDDUpdate
When the Update Automatically checkbox is disabled, RhinoDirect recalculates
the positions of the objects only when you click the Update button.
If some constraints or driving dimensions cannot be satisfied, an error message will appear.
Status Indicator
The color of the status indicator next to the Update Automatically
checkbox reports the following conditions:
-
- indicates that all constraints and dimensions are satisfied. The green light appears following successful recalculations.
-
- indicates that the status of constraints is unknown. In automatic update mode, the
yellow light appears when the model is first opened from a .3dm file. It also appears
when the model is modified by a Rhino command that does not involve a move, rotate, or
drag. When automatic updating is turned off, the yellow light appears after any
geometry or constraint is modified. To update the state of the model, double-click
the yellow light. (Alternatively, enter the LDDUpdate command or click the
button.)
-
- indicates that at least one constraint or driving dimensions is not valid. This light
appears when there is a contradiction between constraints or parameters of driving
dimensions, and so all constraints cannot be satisfied. To make the model
consistent (and change the light to green), remove the contradictory constraints,
or correct the parameters.
Constraints and Driving Dimensions Statuses
Constraints and driving dimensions in RhinoDirect Manager may receive
different statuses depicted by colors
-
green color indicates that the constraint is satisfied.
-
red color indicates that the constraint is not satisfied.
-
black color indicates that it isn't yet known if the constraint is
satisfied or not. Update the model to check the status.
-
grey color indicates that constraint is disabled by user.
You can enable it with Enabled checkbox in the Constraint Properties panel.
Normally in the automatic mode all constraints are satisfied and receive green color.
However, if you create a contradictory constraint which can't be satisfied the
constraint is marked with red color.
Support of Rhino History
You can use the plug-in to control the shape of complex surfaces created with enabled Record History
option (such as extruded surfaces or lofts). To create a parametric loft surface follow these steps:
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Enable Rhino's Record History option and create several profiles (curves or polylines).
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Create a sufficient number of simple objects (points and lines) for each profile .
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Attach the created simple objects to a corresponding profile with help of Rigid Set constraint.
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Specify constraints and dimensions for the simple objects. This way you control the positions of the profiles.
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Create a loft surface for the initial profiles.
Now you can change the parameters of the dimensions to change the position of the profiles.
After the profiles are moved by RhinoDirect plug-in the loft surface is automatically
updated by Rhino.
Note that the surfaces constructed with history are not updated when you animate the model or
use spinner buttons on the Constraint Properties panel. The surfaces are updated only when you
apply the current animation frame to the model or finish modifying parameters with the spinner
buttons.
Animation
RhinoDirect allows you to animate your 3D models by varying the parameters of a
single and multiple driving dimensions.
Single Dimension Animation
To create an animation using a single driving dimension (distances, radii and angles only),
follow these steps:
-
Open the RhinoDirect Manager window.
-
Double-click the dimension you wish to animate, change the animation
parameters by editing their values in the Constraint Properties panel. Animations are
controlled by the following settings:
-
The Start Value field specifies the starting or minimum value of the dimension parameter.
-
The End Value field specifies its ending or maximum value.
-
The Frames field specifies the number of frames for the animation; a
larger number of frames results in a smoother animation.
-
The Time field specifies the duration of the entire animation. Enter 0 (zero)
for the fastest animation possible, which is dependent on the performance of
your computer.
These parameters are stored in .3dm file.
-
Click the Animate... button on the Constraint Properties panel.
(Alternatively, right-click the dimension you wish to animate, and then
select Animate... from the context menu.)
-
Notice that the Animation control panel opens, and that the plug-in
begins to compute animation frames in the background according to
the current animation settings for the constraint.
Animating Multiple Dimensions
You can animate the model by varying the values of several driving dimensions at the same time:
-
Open the RhinoDirect Manager window.
-
Specify Start and End Values for each dimension you wish to animate.
Use the same method as for single dimension animation.
-
Select the dimensions in the RhinoDirect Manager by holding down the Shift or
Ctrl keys. The Constraint Properties panel changes to show just the Frames
and Time fields, in which you specify the required values.
-
To start the animation, click the Animate button on the Constraint Properties panel.
Animating All the Dimensions
Toolbar button: 
Rhino command: LDDAnimate
When the LDDAnimate command is issued, all dimensions are animated according
to the parameters specified by the Constraint Properties panel.
Animation Control Panel (Player)
When single or multiple dimensions are animated, the
Animation Control Panel appears. The panel controls the animation and
lets you navigate through the frames.
The control buttons operate just the way you might expect:
Plays the animation. The direction of the animation depends on which button you click, backwards or forwards.
Pauses the animation at the current frame (available only while playing).
Displays the next frame backwards (or forwards) with each click; to scroll the animation backwards (or forwards), hold down the button.
Jumps to the beginning (or the end) of the animation
You can also drag the slider with a mouse to quickly navigate though animation frames.
Click the Backward checkbox to play the animation in reverse
after the end is reached (cyclical mode). Click the Repeat checkbox to play
the animation continuously, until you click the Pause button.
You can specify the duration of the animation with the Time option.
Enter 0 (zero) to play back the animation at the fastest speed possible on
your computer.
Clicking the Edit... button opens the Constraint Properties panel.
Here you can modify the number of frames, and the start and end values of the
constraint's parameter. Click Apply to apply the changes, or
click Cancel to return to the state before the animation.
About Box and Help
Toolbar button: 
Rhino commands: LDDHelp, LDDAbout
Left-click this icon to open the About Box for the RhinoDirect plug-in. Here you can
find information about the version of the product and your registration details.
Right-click the icon to open the help file. RhinoDirect help can be
also accessed through the Help/Plug-ins/RhinoDirect menu.
How to Register
The RhinoDirect plug-in is on beta stage now. It is not available for registration yet.
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