SOLIDWORKS: Make Part Flexible – How to Modify Components to Allow Flexibility
Flexible Components, first introduced in SOLIDWORKS 2020, allow the assembly geometry to simultaneously drive the geometry of a flexible part. This is very advantageous for situations that require a part to dynamically interact with its surroundings, like a compression spring or even a boot for a shifting mechanism. The ‘Make Part Flexible’ command allows the flexible component to automatically update its position within the assembly without the need to rebuild the assembly each time.
Let’s turn our attention to a specific scenario that extends a little beyond what you might already know. SOLIDWORKS Help is a great online resource to help explain a feature or command. Here you can learn how to change the state of a component in an assembly to become flexible. Maybe you even know how to create your own flexible component. But what about the question; “How do I make my own part flexible? I’ve already spent a significant amount of time modeling this part and I don’t want to have to start all over just because it wasn’t created in the context of an assembly.”
This is a very fair question and one that I have encountered while working support recently. Here, I’ll explain how you can take your own part that wasn’t previously designed to be a flexible component and make necessary changes to take advantage of this capability.
Here is a very quick and basic example of a Bend Tab in an assembly. I just decided that I want this part to update automatically to changes within the assembly. Specifically, I want to emulate a somewhat natural or realistic change in shape for when the smaller plate increases in thickness. Trust me, there are far better and more intricate examples, but this helps to get the point across at a basic level.
My bend tab was not designed to be flexible within an assembly environment. Meaning, I never incorporated a degree of freedom to be in-context with another component. I need to set up an external reference so my part can freely interact with position changes in an assembly. As you can see in the image below, if I right-mouse click or even left-mouse click the part in the Feature Tree to activate the ‘Make Part Flexible’ command, the icon isn’t there. The icon will only be present if the selected component is capable of the characteristic in question.
To address the issue of Design Intent, and allow my tab to portray a bending action, I left the sketch Under-Defined to allow flex at the part’s origin. “Shape-shifting” parts should be designed in a way that allow desired movement without the hinderance of dimensions and relations over-defining the sketch. Sketches for flexible components are not required to be Under-Defined but in this unique case it allows for a neat graphical representation.
Despite my part having the ability to change shape, there is nothing present to drive the shape. That is where the external reference comes in but there is a specific order of operations needed.
A flexible component must be created, or in this case edited, in-context of an assembly. This situation allows the selection of an external reference that ultimately drives the dimension of our part. To accomplish this, first select the part from the Feature Tree and select ‘Edit Part.’
You will now be editing the part in the context of the assembly. The component and all its feature change to a blue text in the Feature Tree and the ‘Edit Part’ Icon displays in the upper-right corner of the graphics area.
The next step, and most important part to remember to do when editing in-context, is to drag the Rollback Bar to the top before the first feature or sketch. Doing this allows us to successfully create a relation between the initial sketch and the reference plane we will now define.
For this example, we want the end of the tab to freely bend in an upward and downward arcing motion as the thickness of the top plate changes. Therefore, the planar face of the top plate will be the selection for our Reference Plane. Use a Distance relation here and set the distance to zero. This zero-distance offset plane acts as a direct replacement of a part face that ultimately moves. This allows for greater control over the placement of the external reference.
Drag the Rollback Bar below the feature containing the sketch that controls the overall shape. In most cases, this will be the first feature of the original part. Then, create a relation between the newly created plane and the portion of the sketch that will contact the external reference in the assembly. In this case, I created a tangent relation between the new plane and the sketch fillet. For additional information about acceptable external reference types, see the SOLIDWORKS Help site accessible through the Help dropdown in SOLIDWORKS.
Exit the sketch and drag the Rollback Bar to the end. Exit the ‘Edit Part’ to return to the assembly environment. At this point you can then select the part from the Feature Tree and the ‘Make Part Flexible’ Icon will now be selectable.
You will now be prompted to engage the flexible component by remapping the missing reference. (Some flexible components may require more than one reference selection)
Here we choose the top face of the smaller plate and we receive a green check in the Flexible references window in the Property Manager. Accept the selection and the assembly component now has a Flexible Component Icon in the Feature Tree as seen below.
Note the automatic repositioning of the part with changed in the assembly.
Upon saving changes, you will now be able to insert this part into other assemblies with the available ‘Make Part Flexible’ command. Simply mate the part into place, select the component from the Feature Tree, and choose the ‘Mark Part Flexible’ Icon from the pop-up menu.
Additional notes regarding capabilities of this feature: While assembly components may be edited in-context, a flexible part cannot.
Should an in-context edit for a flexible part be required, select the flexible part from the Feature Tree again and toggle off the ‘Make Part Flexible’ Icon. Edits can then be made prior to making the part flexible again. Reference selections will prompt once more.
Lastly, when saving assemblies with in-context features, we have the option to save with or without these in-context references. Saving with references requires you to edit the referenced file locations to prevent the in-context features from affecting other instances of the part.
This basic example highlights the overall process necessary for other scenarios to maximize the functionality of a flexible component. Please reference my colleagues blog introducing the update for the 2020 software release if you would like to learn more.
SOLIDWORKS 2020 What’s New – Flexible Components (cati.com)
Thanks for reading and enjoy expanding your dynamic range in Assemblies!
Computer Aided Technology, Inc.