Previously, we created a generic energy chain to give an overview of this great new feature. In this article, we’re going to take a look at a few special use-case scenarios.
Energy Chain with Rotary Motion
The previous example would work great with some type of gantry with linear motion. In this case, what if the motion is more circular or rotational than linear?
Well, it’s all in the sketch path that drives the Chain Component Pattern. You aren't limited to sketches only consisting of lines and arcs for the chain path. You’ll notice that this case requires 3 arcs in the path: one that defines the outer diameter (or the outer ring), one that defines the inner diameter (or the hub), and a small arc that represents the bend or return between the two.
Now in order for this to behave properly, the “dummy” component that contains the chain path sketch must be properly constrained in the assembly. For the correct rotary motion, the component must be concentric to the ring and hub components and, in this case, constrained to the hub so that when the inner hub is dragged (rotated), the chain path moves with it and therefore drives the Chain Component Pattern to move with it. (See below.) Extra features such as bosses and/or reference geometry may be needed in the chain path sketch part to allow you to mate things together as desired.
Closed Loop Chain
Now let’s take a look at a perfect example of a closed loop chain. This one has another interesting twist as unlike the energy chain, which uses a single type of link, a bicycle chain has two types of alternating links.
When we set up this feature, we’ll need to pattern both the Inner and Outer Links that alternate to make the chain. We’ll use the “Chain Group 2” option and selections to accomplish this.
Something else to consider here is that in reality, the final link in the chain would be attached to the first link in order for it to be a closed loop. However, we cannot create the mate to accomplish that in SOLIDWORKS. So, how do we make sure the total length of our path is correct so that the final link does indeed meet the first one?
The trick here is to determine the total number of links you want and use the “Fill Path” option. Once this is done, you can measure the remaining gap between the first and last component. Using the Path Length Dimension, adjust the sketch path by that amount to close the gap.
In-Context Chain Path Sketch
There are applications where the movement of the chain is dependent on the position of other components in the assembly to which the chain is attached. This is easily done by creating an in-context sketch constrained to the moving component, in the chain sub-assembly.
In this example we have a gantry system where the chain path sketch is defined in the context of the assembly to the vertical head component. Notice the angle of the path is not specified; it is dependent on the position of the head component.
Now, there is one difference in the behavior of the chain movement when using in-context referencing for driving the chain path. When the component (the head) is moved, the chain motion will not be real-time. The top level assembly MUST be rebuilt so that the chain path sketch is solved for the new location of the component, which then allows the chain component pattern to be solved. This is still very useful for positioning information in your design and drawings.
In part 3 of this series, we’ll take a look at special considerations regarding optimum behavior and performance when using the Chain Component Pattern in SOLIDWORKS 2015.