In this guide, learn how to create a custom Library Feature Part. Some advanced topics are discussed toward the end.
First, make a base feature on which you will create the features you want. You’ll want this to some-what represent what the LFP will be used on. i.e., jetted ports go on the end of a cylinder, so make a cylinder as your base. In this case, since it’s sheet metal, we will use just a flat piece. It doesn’t need to be anything special.
Create the shape and features you want. Dimension it with design intent. In this case, we want the center of the circle of the keyhole, so I’m aligning that with the origin. I want a lip on it. You’ll want to use construction lines a lot here. They can be used to adjust insertion points and be used for alignment when you insert it into a new part.
Once you’ve created the feature you want, you’ll need to select the features you want to “copy and paste” into any design. See below image for clarity. Use “CTRL + Left Click” to select all the features.
IMPORTANT: If you are making things like through holes, make sure you’re using “through all” or extrusions that terminate at a non-standard face (like, not just .1in, but a variable face) utilize “up to next” or “up to surface”. These features are 100% design intent. You’ll need to consider what happens when it’s inserted!
Then, with the features highlighted, press Save As. Save the features as a Lib Feat Part (.sldlfp).
You’ll need to save it in a location that you can see. Adding a design library location can be shown in our video here: https://www.youtube.com/watch?v=53MVWWpoQqE. Yes, you can put whole parts in there!
These features should now have an “L” next to them to show they are Library Feature Parts (LFPs).
You should now also have a references and dimensions folder. These can be edited (and configured!), and references can be added. You can get really complex here, so I’m going to leave it at this stage of the guide with a few notes later on.
After that’s set up, drag and drop into the new design.
It will be undefined until you give it a reference. Like a point! To avoid this being a common problem: go back into the LFP and remove the reference. Remember to resave the LFP! This will make it drag and drop with no restrictions, but it won’t be easily locatable.
Some additional tips
Reference Dimensions
If you reference the “outside” (the base plate), you can utilize those dimensions as “Locating Dimensions”. This will insert a reference onto the future design automatically. This is most common to locate where it’s going in space. If I remove the “Origin” snap, and use any dimension to locate it, when inserting the LFP it will automatically request to find an edge referencing that dim.
Like so, see my “throwaway” dims of 2.52 and 2.26 here. They don’t need to be accurate; they just need to exist.
You will need to move these into the “Locating” file. Simply drag and drop.
Inserted into new design…
It prompts for the bottom edge. And the right after satisfying the first reference. You’ll see a green check if it’s okay. You can use this to rotate or align.
Editing, Resaving, and File Maintenance
Editing can be tricky. You’ll need to save it to a new name every time. You can go back and rename the file in post. I actually messed up and made a “2” and then renamed it back to its original name after deleting the first one. These are not like normal SOLIDWORKS files. They can be renamed and moved. As long as the folder is specified like the video earlier, you’ll see them.
Remember to back these up! Upgrades, and reinstalls can wind up deleting these locations. Personally, I recommend creating a common location for these to be saved that can be easily moved/saved/recovered if need be!
Configurations
You may have noticed on insertion, that configs are possible. Utilize them for features that have variable size! You can create configs like normal in the LFP file. You can go wild and use equations. As you can tell, you can really do a lot with these, and this guide could go on forever! Try some stuff out.
Not working like it should?
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