solidworks tipsWouldn’t it be nice to automate all the modeling you do in SolidWorks? There’s ways to do this but when you’re first implementing SolidWorks or need to add some methods to speed up model creation there’s a way to make adding features quicker. It’s through Library Features and this will show you what they do and tricks for the best way to do it.


What’s in blazes is a Library Features?
Let’s open up the SolidWorks chest cavity and see what’s inside. A library feature is a file that contains features. It’s a quick way for you to save features you use a lot. It helps you create parts and maintain consistency. In its simplest form, it’s a hole you use everywhere and drop it in when you need it. The alternative to this is tediously starting a sketch, sketching a hole, cuting a hole – over and over.

You can imagine how this would help if you had a more complicated feature.

A Library Feature looks like a normal part, but the FeatureManager shows you the lucky items you have selected to be part of the Library Feature. You can do this for most features you create… but how???

The absolute best way to create Library Features and get them to work
Library Feature can be tricky little suckers. You’ll drop them in and something doesn’t work quite right. This is where we give up and go for a drink… or try and figure out what’s wrong.

It may be useful to go ahead and download the files for this so it’s easier to understand what I’m talking about. You can even use the example library feature as a starting point for others. These tips below assume you have a base part started and your ready to make your feature.

Create a positioning Sketch
This is the crucial component and does two things. One, it reduces the amount of relations you need to locate the Library Feature when you drop it in and two, it’s the foundational element for the rest of the Library Feature. Select the face and draw an two perpendicular lines with the centerline tool. Delete the relations and add just one relation to make them perpendicular. Don’t lock them down to a point or anything else. You want this sketch to be as flexible as possible.

Create some locating planes
This will give you two planes to help locate parts that use the library feature, like a tab going in a slot. These planes make it easier to mate them together, plus if you have an ace of a programmer, you can even automate it. Here’s where the positioning sketch first comes in handy. First, create a plane with a distance of zero off the face. Using that plane and the sketch lines, create a couple angled planes.

Keep features simple
This is extremely important and what usually causes problems.This means as few dimensions and relations as possible. Relations can be the toughest, because a lot of them are added automatically. I will usually create my sketch, blow away all relations and add just the ones I want. The example uses four holes, dimensioned to the positioning sketch.

Center features if possible
This will make them behave better. It has a lot to do with how the library feature is being used. If you make a part or assembly that is nice and symmetric, it’s pretty easy to figure out how the Library Feature should be made. If it’s not symmetric you may have to test things out a bit and see what works best. This shows how important it is to create assemblies and parts for how you need to use them to get your work done. If all else fails start with building in symmetry.

Save the Library Feature
In your part file, select File, Save As… and select Lib Feat Part (*.sldlfp) in the Save As Type pulldown. In the FeatureManager right click the feature and select Add to Library. If you right click again you can select Remove from Library to remove it. I’ll add here that it’s extremely useful to have a your team organized. I add it to a common network location and set up a folder in the Design Library on the SolidWorks Task Pane for all my Library Features.

Create some Templates
This way you won’t have to start every library feature from scratch and if there’s a lot of people making them, you’ll keep the Library Features more consistent. It also saves a lot of time explaining (see above) the process of creating a Library Feature.

Test it out
Now you’ve got a Library Feature. Test it out by dropping it into the part. Make some adjustments, save and test again. You can see how to test it in the video below. I start with creating a sketch that my library feature will be positioned by. Go here to see it in HD.

This kind of stuff goes beyond the everyday modeling type stuff, but hopefully it’s given you some insight into ways you can reduce some of your effort. When I see something that would be a good candidate for a Library Feature, I usually pause because it can take some time to think it out. The above tips make it easier for me and I’m hoping for you too. Here’s the files one more time.

SolidWorks Library Feature Files

What about you? Do you use Library Features?


Josh is founder and editor at, founder at Aimsift Inc., and co-founder of EvD Media. He is involved in engineering, design, visualization, the technology making it happen, and the content developed around it. He is a SolidWorks Certified Professional and excels at falling awkwardly.