SOLIDWORKS Design Library - Custom Library Features
In this article, I’ll explain how to use, create, and test custom Library Features. If you’re unfamiliar with Library Features, you can use them to insert commonly used features into your designs. They save time by reusing design time whether you develop your own custom features, or you use the default options installed with SOLIDWORKS.
Using the Design Library Features
To use a Design Library Feature, start by expanding the Design Library folder structure to the features folder. Then expand the features folder.
Select and expand the standard or type of feature and select the required feature. Next, drag and drop the Library Feature onto the solid and follow the directions.
Here is a short excerpt from the SOLIDWORKS Essentials – Configurations – Lesson 10:
Creating Custom Options
To create a custom library feature you need to start with a part that contains a base feature. Depending on the shape, the basic solid will be rectangular or cylindrical. Here we will start with one of each.
Custom Rectangular Library Feature
Starting with the rectangular base, I have created a simple cut feature, like this.
Renaming the variables that define the Length, Width, Depth, and the x/y position of the cut will help define the future references of the library feature.
Next, select the Cut-Extrude1 feature and open the design library tab from the Task pane. Now, click on the Add to Library button (shown here)
This will open a dialog to create a Lib Feat Part (*.sldflp), which I’ve named RectangularCut.
This will add the library feature to the design library in the file location you chose:
Now we need to open the library feature from the design library to manage the references. The placement references will be inserted into the References folder and the dimension variables into the Dimensions folder at the top of the Feature Manager Tree. The locating dimensions Loc_X and Loc_Y will need to be dragged into the Locating Dimensions folder. Be sure to drag any dimension you don’t want to show in the Library Feature Property Manager into the Internal Dimensions Folder.
To test your rectangular feature, create a part with an extrude then drag and drop it from the Design Library.
Custom Cylindrical Library Feature
Now, when creating a round or revolved Library Feature there are things you will need to decide about the design intent.
- Will it be located concentric to another feature?
- Will it be located using a sketch point (similar to the hole wizard)?
- Will it be located with dimensions (in this case you can use a rectangular base)?
When creating the sketch for the library feature be sure and create references within the base feature. Avoid the origin unless you will be using a sketch point as the location.
Here I have created a revolved cut that can be located using a circular reference.
- A sketch was created on the top face of the cylinder with a construction line that starts concentric to the Base feature, going horizontal past the edge of the base, then the sketch is renamed “Drop location”.
- A plane is created from the line and the end point of the Drop location sketch.
- The revolve profile is created on the new plane with coincident relations to the Drop Location sketch.
NOTE: Try and avoid creating any sketch relations to the Origin. These will add a sketch point requirement for placement of the library feature.
Now, follow the same process as before for adding it to a file.
To test your Revolve Library Feature, create a part with a cylindrical extrude. Then drag and drop it from the Design Library.
Adjust the Size Dimensions to get the shape you need.
I hope you have gained a greater understanding of Library Features and will create your own to speed up your design process.
We’ve covered some additional best practices for how to use Design Features to speed up your design process in a prior blog post.
Dennis Barnes, CSWE
Sr. Applications Engineer, Software Solutions
Computer Aided Technology