| Tutorials
RhinoWorks Basic Tasks: Assembling and Animation
Here is a simple tutorial which shows how to start playing with RhinoWorks plugin for Rhino. The goal is to show how parts can be assembled together into a simple 3D-model providing a possibility to easily control the final shape.
To start with this tutorial ensure that the plug-in is properly installed and you see this RhinoWorks toolbar among other Rhino toolbars (see how to install here).
If everything is OK with the plug-in installation, via Rhino's menu File/Open open the Pantograph.3dm which can be found in Samples folder of the plug-in installation directory or can be downloaded from our sample models page .
Click on 
icon to open the RhinoWorks Manager panel
which contains a list of existing constraints and dimensions, now it's empty.
For the moment disable the Update Automatically check-box on the RhinoWorks Manager panel. It means that the application of created constraints and dimensions will be done only on the user request. Also enable Assembly Mode check-box. It will ensure that RhinoWorks does not change the geometry of the parts, only the position of the parts will be changed.
We will consider the blue part as a base (anchor) of our assembly, let's fix it by clicking
icon and then selecting the blue polysurface in the working area.
Hit Enter to confirm the creation of the fixation constraint.
"Fixation 1" constraint appears in the RhinoWorks Manager. Double-click it in order open Constraint Properties panel.
Then, start assembling the parts with creation of a Concentricity constraint. Click 
icon. Select the pin surface and the hole surfaces to make them
concentric as shown on the picture.
Then create three other Concentricity constraints for other pairs of pins and holes. To repeat the same Rhino command you can right-click anywhere instead of clicking its icon every time. Four Concentricity constraints are now shown in the RhinoWorks Manager.
Let's see what we've just done. In order to apply the constraints and update your geometry
click 
icon. All pins and holes are now really concentric (their axes coincide).
However, there is an intersection between the parts. Let's get rid of it by creation of Coincidence constraints for the planar faces of different bars.
Enable the Update Automatically check-box on the RhinoWorks Manager panel. Now all constraints and dimensions are applied automatically as soon as they are created.
Click on 
icon and select the top planar face of the green
pin and the top planar face of the red bar. Coincidence constraint will be created between these
faces. It will be applied automatically making the planar faces coincident.
In the same way create two other Coincidence constraints between the red and the blue parts and between the green and the magenta parts.
OK, now there is no more intersections between the bars.
By clicking 
icon create the Angle dimension in order to control an angle
between the bars. While creating the Angle dimension select the planar face of the red bar and another planar face of the blue one.
Type "C" when asked for the command options and hit Enter in order to specify an axis for angle measurement (there is a better control of an angle dimension when an axis is specified). Select the cylindrical surface to be an axis.
Hit Enter when asked for angle value in order to take the current one (this value is computed from the current geometrical position between the parts).
Now your model is finally assembled, also there is a possibility to easily control the angle between the bars.
Modify the angle parameter in order to obtain different configurations of your model. If the Constraint Properties panel isn't shown double-click the "Angle 1" constraint or do right-click on it and then select "Edit.." from the context menu. On the Constraint Properties enter "45" in the Value field and hit Enter.
The geometry of the assembly will be updated automatically, the bars will be rotated and moved according to the changes of the angle dimension.
You can also analyze the kinematics of your model by animating it with changing the angle parameter. To do that enter "45" and "120" into the Start Value and the End Value fields of the Constraint Properties panel respectively. Then hit "Animate..." button. Animation panel appears.
To watch the animation click the right side
of 
button. After the animation is stopped try to drag the slider back and forth, see
how model is changed.
In order to modify the bounds for the angle parameter click the "Edit.." button and enter new Start and End values for animation into the corresponding fields of the Constraint Properties panel. To have more smooth animation you may also increase the number of frames. Press "Animate..." button on the panel to animate the model with new parameters.
Play more with this model, try different values of angles. Try to remove existent constraints and introduce other constraints and dimensions.
Advanced Tutorials on RhinoWorks
How To Make a 3D Cartoon in Rhino
How to Express Design Intent in Rhino 3D
Part I. Assembly Design and Kinematic Simulation
