By Ben Taylor
Some people consider me lazy, but I prefer to be called “strategically efficient”. I don’t like repeating the same task again and again, so I use automation tools like Library Features to do the work for me. Library Features can be a sketch, a single feature, or a series of features that are used frequently. They need to be created once and then can be saved to the Design Library to be used repeatedly. In this article, I will be looking at tips on how to create a SolidWorks library feature. More specifically, I will be creating a solid body within a weldment multi-body part by using the Library Feature capabilities. As shown below, I will walk through creating a Library Feature to quickly add a bracket with holes to a pair of structural members.
Here are the basic steps to creating a solid body from a Library Feature: 1. Create the intended feature with all of its requirements (sketches, planes, etc) within a “dummy” part. The part itself does not need to be saved, but should accurately represent the part in which the Library Feature will be repeatedly used in the future.
After creating two joining structural members as the “dummy” part, I start my Library Feature by creating three planes: Side Plane1, Side Plane2, and Mid Plane. Planes 1 and 2 both have zero offsets from the highlighted faces, while Mid Plane is centered between the top and bottom face of the members. These planes will make more sense in the next few steps.
The sketch for the Left Bracket Tab feature is created on Side Plane 1, not on the face of the structural member. I find that Library Features with multiple sketches work better when the sketch is placed on a plane within the Library Feature, not an external source. Some important TIPS:
A. Build in as few external relations as possible. You can quickly lose efficiency here, as every external relation has to be assigned when the Library Feature is inserted into a new part. Also, these external relations can be a source of errors. To keep it simple, I only created relations to the planes within the Library Feature. This maintained all the external relations linked only to the three planes
B. Avoid sketch relations like vertical and horizontal, as these relations will realign to the new part’s coordinate system. This may provide unexpected results and makes it difficult to orientate the Library Feature at different angles
C. I initially tried extruding an “L” shaped sketch from the Mid Plane, but found it hard to avoid external relations and the Library Feature would create the solid body in undesired locations. That is why I chose to create two separate extrusions from the side planes. Library Features may not be difficult, but will often require multiple attempts
The remaining features are then created.
A. Again, try to avoid any external relations. For example, the ¾ Clearance Hole is a blind cut, not an up to face end condition
B. Keep it simple. An excellent motto to live by when dressing yourself for a street fight, writing lyrics for techno, and for creating Library Features. The more relations, sketches, features, planes, etc. that you place in your Library Feature, the more that can go wrong and the longer it can take to setup/orientate in the new part.
C. Configure the features and dimensions, if required. Any configurations within the part will be available when dropping the Library Feature. For cases like Weldment parts, you may need to remove configurations (As Welded and As Machined are automatically created and may not be needed)/
2. Save the Library Features
- Hold down the Ctrl button and select all the sketches, features, planes, etc that you wish to include in the new Library Feature. With only these items selected from the Feature Tree, go to Files-> Save As and change the Save As Type to Lib Feat Part (*.sldlfp).
- You can use Windows Explorer to later drag and drop the Library Feature into a part, but I personally find it more convenient to have the Library Feature location available in the Design Library. Consider this when choosing a save location
- Once the Library Feature is saved in SLDLFP format, the “dummy” part can be closed (it does not need to actually be saved as an SLDPRT part file)
3. Drag and drop the new Library Feature into a test part
- As mentioned earlier, creating a proper Library Feature may require several trials. Be sure to do ample testing and start simple. If you share your new creation with your coworkers before proper testing, they may find errors and lock you in the broom closet. Again.
- When you drag the Library Feature from the Design Library, or Windows Explorer, I suggest NOT dropping it on the part. Rather, I recommend dropping it in the blank graphics area, close to its intended location. If you drop the Library Feature on a face, it will use that face for the first reference (see the next step). Unless you know the Library Feature extremely well, this may cause issues.
- After dropping the Library Feature, the Property Manager will ask you to choose a configuration, any required references, and dimensions for locating and size. A preview window with the “dummy” part and Library Feature will also pop up to help guide you with the reference selection.
- The highlighted reference geometry in the “dummy” part preview window is asking you to select the matching reference geometry on the new part. Also, the reference box in the Property Manager lists the required references- references with a “?” next to it still needs to be assigned, while a green check mark says it has been assigned.
Once you have fully tested the Library Feature and feel confident that it does what it should, make sure to share it with your coworkers and allow them to buy you cake. Enjoy!