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Using Dynamic Spline Curves

B-Splines are the most familiar type of spline in Alibre Design and are useful for a wide variety of tasks. However, one of the strengths of B-Spline curves can also be a weakness in certain circumstances: they are rigid and not subject to changing shape without explicit intervention. This lesson covers how to make another kind of spline – a Spline by Reference Points – which allows your spline curves to change shape as your part or assembly changes without manually changing the points. If this is what you are after, it can save you a lot of time, and allow some pretty neat tricks such as dynamic cabling in an assembly for example, which we’ll show in this lesson. Though this lesson shows only a cosmetic example of the use of this tool, often this method works whenever you need a flexible spline curve.

1. First, we’ll create a new assembly and insert a new part to begin our design. We’ll be designing a cabling system, so we’ll need 3 parts: 2 connectors and the cable to go between them. We’ll start with the connectors. Below, we’ve modeled an example connector piece.

2. Now, we’ll duplicate the connector we just made and insert it opposite the original. To do so, right click on the new part in the Design Explorer and select Insert Duplicate. You can now begin placing as many copies as you need. We need only 1.

3. In our example, these two connectors face each other and lie on the same line. We’ll need to constrain them to behave in this manor. First, we’ll use the rotate and move tools to reorient the second connector in the approximate position it should be in. Then, we’ll begin by applying an align constraint to the two cylinders shown below.

4. Now, we’ll apply another align constraint to the two cylinders shown below. This leaves only one degree of translational freedom for our assembly, basically allowing only the to-and-fro motion simulating the connectors getting closer or farther from each other.

5. Now, we’ll make the dynamic cable. We’ll need to create a new part and use the existing geometry of the two connectors as the starting and ending points of our flexible Spline by Reference Points. To do this, we’ll use the Project to Sketch tool. Below, we’re in a new Part Workspace within the context of our assembly and we’ve entered Sketch Mode facing the sides of the connectors.

6. Now, we’ll use the Project to Sketch tool to bring the existing connector geometry into this sketch, and we’ll select “Create Reference Figure” and “Maintain Association to Source” to ensure that when we move the connectors in the assembly, it updates this sketch as well so our cable changes with it. We’ll elect to use Reference Figures because these will not actually be part of our sketch. We’ll be projecting 4 items – the ends of both tubes and an edge of the faces the tubes touch.

7. Now, we’ll create 3 figures – 2 lines which represent straight portions of the wire that go inside the connector and a Spline by Reference Points that connects to those lines, representing the “stretchy” portion. The layout is shown below, and the blown up portion shows a simplified version. This sketch will act as the path for a Sweep Feature. So, the next step will be to make our profile for the Sweep. Spline by Reference Points is located within the menu structure under Sketch > Figures > Spline > Create > Spline by Reference Points.

8. We’ll get out of this sketch and we’ll make a new sketch which will represent our profile for the Sweep Feature. We’ll enter sketch mode on the face highlighted below and we’ll create a circle concentric to the connector’s circle, equal to the inner radius. To do this, we’ll simply project the inner circle of the connector piece using Project to Sketch.

9. Below we can see the result of the circle that is created when we Project to Sketch the inner circle of the connector piece. We’ll check Maintain Association to Source and we’ll create a Sketch Figure instead of a Reference Figure. Now, we have a path and a profile – it’s time to make the Sweep Feature.

10. Generate a Sweep using the Sweep Boss feature, using the first sketch we made as the path and the circle we made as the Profile. The result is below – you can see that the ends within the connectors are straight due to that portion of the profile being a line, and it fits perfectly. Even if we change the size of the holes later, the wire will update automatically because we chose to Maintain Association to Source. The next step is to pattern this wire since we have 3 total connections to make.

11. We’ve made a Linear Feature Pattern to accomplish creating more wires. Depending on what you’re doing, this could work or may be the improper way of doing things. We’re considering the 3 wires to be a single unit. If your application were to require them to be counted separately, the proper method would be to use an Assembly Pattern. Regardless of which type of pattern you use, the advantage is that you don’t have to constrain each item again. Now, we’ll get back into the Assembly Context so we can start moving the connectors and see what happens.

12. Now, when we move the non-anchored part (bottom left) the cable updates in real time and the wire gets longer. It’s important to note that this kind of operation (Sweep) is pretty expensive in terms of processing power for real time updates, so it’s a good idea to keep instances of it to a minimum. If you want to get extra fancy, or extra precise, you can create relationships between the reference points of the spline to make it bow or flatten depending on how far apart the end points are from each other – something which we will not cover in this lesson. By default, only the endpoints of the spline move, so you would need to set up some additional relationships on the reference points of the spline if maintaining a precise shape is important to your application.

In this lesson, we’ve covered the specific use of how to use a Spline by Reference Points as a way of creating flexible cabling. However, the more important lesson we’ve run though centers on how to create dynamic items in general, regardless of whether they employ Splines. The general workflow is to use Project to Sketch to re-use reference geometry from existing parts as the basis for new parts. When you use the Maintain Association to Source option, which you should do intentionally and not out of habit, your new parts automatically update their size or location when the source geometry’s size or location changes.

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