Hello, this is Jackie Yip with Alignex. With the SOLIDWORKS 2020 release, making a part flexible is one of the amazing new features that allows your parts to modify in real-time with the motion of an assembly. And with it – the same part can be reused in other assemblies without the need of separate configurations. If you’re looking to optimize the flexibility of your parts with less rework required in the model, then this will be a great tool for you.
In the following example, we’ll need the create an assembly with the two plates to control the flexibility of the spring. I’ve already created this ahead of time and simply created an extrusion of a circle, adding another instance in the assembly and with the concentric and parallel mates, the plate can now slide up and down. Now it’s time to make a new part for our spring. To control the flexibility of the spring, we’ll leave a portion of the setup under-defined and this will require to use of the sweep feature. Both the path and profile sketches will be drawn on the front plane with the path sketch under-defined. Next, I’ll go ahead and insert this part into the assembly and use a couple of mates to align the centers.
Before applying the sweep feature, I’ll be editing the part in-context and then rolling back the tree before the two sketches. Then I’ll add a new reference plane to the bottom face of the top plate. Once the tree is rolled forward. I’ll edit the path sketch to apply a coincident relation from the endpoint to the plane. The plane will now act as the external reference that’ll control the flexibility of the spring to wherever the plate is re-positioned.
Finally, we’ll select the sweep feature to pick the path & profile. Under advanced options, the profile twist options will generate the preview of the spring. With a few finishing touches, we’ll now return back to our assembly and simply drag the plate and then press rebuild to flex the spring.
With the external references setup on the spring, we’ll now introduce a powerful feature to make this part flexible in any assembly. If that doesn’t sound convincing, let’s briefly explain how this feature works in SOLIDWORKS 2020. We’ll need to have a second assembly in order to do this, so I’ve already created a new assembly with two square plates. Next, we’ll insert our spring and then add a couple of coincident mates to get it properly positioned. Now for the surprise, we’ll simply click on the spring on the Feature Tree and select Make Part Flexible. This new option allows us to remap the external references to the new part in this assembly. I’ll select the bottom face of the square plate which will now follow the position of that component.
Let’s take a closer look at our assembly, the new flexible icon appears next to the spring. Notice that our spring automatically rebuilds when dragging the plate. Future assemblies can now control the flexibility of the spring independently without the need of an extra configuration. With making parts flexible in SOLIDWORKS 2020, it delivers in saving design time as more versions of the same part are no longer necessary.
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Written by Jackie Yip
Jackie Yip is an Application Engineer at Alignex, Inc. When Jackie isn’t assisting customers on the Alignex Help Desk or teaching a SOLIDWORKS Essentials class, he enjoys road biking and keeping up on the latest tech trends.