Using the Design Library and Smart Components

One of the greatest ways to save time in SOLIDWORKS is to create and manage a design library of features. Let’s say there’s a cut extrude you need to use over and over again on different models. This cut extrude can be saved as a “design library feature” and stored in a library so that it can be easily accessed and applied again in future designs.

A Simple Example

Let’s say we work for a company that designs guitar amplifiers.

Figure 1. Let’s say we work for a company that designs guitar amps.

Each guitar amp is a little different, but they all have one thing in common: they all need power. A typical power supply for these amps comes in the form of a 3-prong power port on the back of the amp, as shown in Figure 2.

Figure 2. A typical power port found on the back of an amp.

The power port shown in Figure 2 will require a rectangular cutout, some fillets on the corners, and two holes for the mounting screws.

Figure 3. The back of our amp which does not yet have the required features for the power port.

When we examine the back of our amp and we see that we do not yet have these features, we could begin a new sketch and cut extrude a rectangle, then add fillets in the corners, then add the two holes for the mounting screws. However, we would have to do this for every amp we design which would amount to a lot of repetitive work. This would be a great opportunity to use a design library feature.

A Design Library Feature

A SOLIDWORKS Design Library feature is a library element that consists of one or more features which can be dragged and dropped onto a new part. In the example below we have constructed a design library feature which consists of three features: a rectangular cut extrude, the corner fillets, and a cut extrude for the mounting holes.

Figure 4. The three features of our design library feature.

Once we have built this design library feature, we can drag and drop it from our library onto the desired part. In our example, we will edit the back plate of the amp and drag and drop the library feature, as shown in Figure 5.

Figure 5. Dragging and dropping the design library feature.

Once we complete the drag and drop, we will be asked to select a horizontal edge and vertical edge to define the location of the library feature, as shown in Figure 6. This is due to how we defined the library feature when it was created, and we will examine this concept in more detail in just a few moments.

Figure 6. Defining the edges for the library feature.

Once the design library feature has been dropped onto the back plate and these edges have been defined, we can hit the green checkmark to finish adding the library feature to our model.

Figure 7. The tree now shows the library feature and nested features. The locating dimensions can be adjusted.

The library feature will now appear in the feature tree and the three sub features will appear nested, under the library feature. The dimensions controlling the location of the library feature will be defined to the horizontal and vertical edges we selected earlier, and these dimensions can be adjusted as desired.

We have now successfully added a design library feature to our model. The great thing about design library features is that once you have created the library feature and added it to your design library, you can apply it over and over again. In our example, we have a line of 20 different guitar amps. Each amp has a common feature (a power port) and we now have a library feature that we can use on all 20 of these amps.

Creating a Design Library Feature

Now that we have shown how to use an existing design library feature, let’s show how to create a new design library feature. Most of our amps require a series of slots on the back panel to promote ventilation and airflow. We will now create a new design library feature representing these slots.

Create a Dummy Part

The first step in creating a design library feature is to create a “dummy part.” This part is typically a simple extrusion. The purpose of the dummy part is to act as a place holder that will eventually be replaced by the actual production part. In our example, we will create a dummy part as a rectangular extrusion, and when we drag and drop our library feature (the slots), the dummy part will be replaced by the rear plate of the amp.

To create our dummy part, we simply begin a new part file and sketch a rectangle. The size of this rectangle is not important, but it should approximately measure to the average size of a back plate of our amps. Since our back plates range from 1.5” x 8” x 0.090” (on our smallest amp) to 4” x 24” x 0.090” (on our largest amp), we will create a dummy part that is 2” x 14” x 0.090”.

At this time, there is nothing special about this part. It is simply a new part with a single boss extrusion, as shown in Figure 8.

Figure 8. The dummy part has been created with a simple boss extrusion.

Adding the Library Features

We will now repeatedly add the features we wish to use. These features will be a rectangular cut extrusion (the first vent slot), four corner fillets, and a linear pattern.

We begin with the first cut extrusion. We will select the FACE (not plane) of the dummy part and begin a new sketch.

We will begin with a corner rectangle and we will place it near the far right side of the model. We will add dimensions to the right edge of the dummy part, the top edge of the dummy part, and the bottom edge of the dummy part, as shown in Figure 9. We will also add a dimension to the width of the slot.

Figure 9. The rectangle for our first slot has been dimensioned to the three edges of the dummy part.

Adding the Remaining Features

Next, we do a CUT EXTRUDE of this rectangle, and then add a small R0.015” fillet to each of the four corners. We will then perform a linear pattern of the cut extrude and fillet features, giving us a slot pattern.

Figure 10. The dummy part with three features which we wish to turn into a library feature for our vents.

As we can see in Figure 10, the model is still a standard part file which consists of a “dummy part” (Boss-Extrude1) with three additional features which we wish to turn into our design library feature.

Turning a Standard Part into a Library Feature Part

To add our three features to the design library, we begin by selecting them from the feature tree. We can do this by selecting “RECT Slot Vent,” then holding CTRL and selecting “Corner Fillets of VENT” and “LPattern-Vent Pattern.”

Figure 11. Holding CTRL and selecting the desired features.

Next, we can go over to the SOLIDWORKS DESIGN LIBRARY tab of our TASK PANE and choose ADD TO LIBRARY, as shown in Figure 12.

Figure 12. Selecting the design library and choosing ADD TO LIBRARY.

After clicking ADD TO LIBRARY, we will be presented with the Design Library property manager, as shown in Figure 13.

Figure 13. The Design Library Property Manager.

When creating a new Design Library Feature, we’ll be asked to choose the features we wish to include. This should be every feature except the “dummy feature,” which was “Boss-Extrude1.” Next we’ll be asked to give the library feature a name. Lastly, we will be asked where we would like to store the library feature in the Design Library. The default “Features” folder shown in Figure 13 is a good location for your first design library feature, but eventually you should create your own custom folder.

Once you have specified the features to add, the name of the library feature and the location for it to be saved, hit the green checkmark to complete the creation of the Design Library feature.

A “Special” Part File Type

You have now created a special type of part file: a “Library Feature Part File” with the extension .sldlfp. The part file now has a special icon at the top of the tree, as well as two new folders (REFERENCES and DIMENSIONS). Also, some of the features in the tree now have a little “L” symbol on their icons. As shown in Figure 14, this is to be expected when creating a new library feature part file.

Figure 14. The special features that appear when working with a library feature part file.

Using Our Design Library Feature

Now that we have created a design library feature we can add it to our model. We created a series of slots to help with airflow in our amp, so let’s try to add this feature to the rear plate of our amp.

We begin by closing the library feature part we just created and then returning to our assembly. If you are asked to SAVE, you can say NO. Next we make sure that we are in edit part mode, editing the rear plate, and that we can see the “VENTS for rear of AMP” feature in our SOLIDWORKS Design Library.

Figure 15. Preparing to add our vents to the rear plate of the amp.

As we can see in Figure 15, we have successfully located our library feature part. We now drag and drop this feature onto the rear plate of our amp.

Figure 16. Drag and drop VENTS library feature.

When dragging and dropping the library feature, the preview may appear as though the vents are too large for the rear plate. No need to worry though. If you recall, when we created the sketch for the vents (in Figure 9) we added dimensions to the top, bottom and right edges of the dummy part. These edges become “missing references” in the new part when we drag and drop the library feature. So we are now prompted to re-establish these missing references and, when we do, the slots will automatically resize to the current version of the rear plate, as shown in Figure 17.

Figure 17. Selecting the three “missing edges” from the dummy part to be replaced by three edges on the rear plate.

We have now added the library feature to our model and it looks pretty good. But if any of the dimensions for the slot width, height, number of slots or slot spacing needed to be changed, we could simply select the library feature from the rear plate and make the desired adjustments.

Figure 18. Adjusting the dimensions of the slots.


Using Smart Components

In our thorough review of how to use Design Library features in SOLIDWORKS, we were able to use a library feature to create a rectangular hole for our prong power port, including the 2 holes on the sides for mounting hardware. From here we could certainly bring in the three-prong power port, screws and nuts, and begin assembling them.

Figure 19. Adding the assembly components and mating them together

So yes….we could add these 5 parts to our assembly and add mates to them to get them into position. But that seems like a very “manual” process. It seems like there should be a more automated way to use and reuse this common setup, from one assembly to the next, similar to using design library features.

Well, there is indeed a way, and it is known as utilizing a “Smart Component”.

Creating a smart component

Let’s take our assembly to a point where we still have the slots, but no longer have the hole for the power port. The slots work GREAT as a library feature, because the slots are a single group of features.

The power port, screws, nuts, and rectangular hole and mounting hardware holes, on the other hand, would be a great fit for creating and using a SMART COMPONENT…especially since we plan on using this same setup on many different assemblies.

To get started we’ll get rid of the design library feature we created earlier, in our model.

Figure 20. We no longer need the holes for the power port

Next we are going to once again create a dummy part. Again a rectangular plate representing the average size of the rear panel of the amp (14” x 2” x 0.090”). This time we are going to SAVE this dummy plate as a standard part.

Figure 21. We create a new “dummy plate” and save it as a standard part

Now we will add this “dummy plate” part to an assembly, along with the 3 Prong Power Port, two screws and two nuts. We will save this assembly as “SC-1.sldasm.”

Figure 22. Our Assembly, containing the dummy part, three-prong power port, and mounting hardware.

Next, we need to mate our components into place using a coincident mate and two distance mates.

Figure 23. Our Assembly with distance mates to the edges of the plate.

Next, we are ready to add mates to our assembly for the remaining hardware. We will mate the hardware to the front face of the power port and the rear face of the dummy plate.

Figure 24. Our Assembly with hardware mated into place.

At this point we have all of our common components mated to the dummy plate, but we have no holes going through the dummy plate for the power port or the hardware. To create these cutouts, we will begin by saving the assembly and then choosing EDIT PART on the dummy plate. Once we are in EDIT PART mode, we will begin a new sketch on the front-most surface of the dummy plate.

Figure 25. Edit the dummy plate and begin a new sketch on this surface.

Once we are in sketch mode, we will use CONVERT ENTITIES to convert the edges of the holes for the mounting hardware. We will also select the edges of the rear area of the power port and choose to convert these edges into the current sketch so that our sketch looks similar to Figure 26 below.

Figure 26. Convert the edges of the holes and the rear of the POWER port to create this sketch.

Now we will take this sketch and perform a cut extrude (up to next) on the dummy part. Similar to a library feature, this cut extrude will be used and reused anytime we drop our smart component.

Figure 27. Adding the cut extrude to our dummy part (with other parts hidden for clarity).

We now have our dummy part in an assembly. We have our corresponding parts (our mounting hardware) and an in-context feature (our cut extrude). We are ready to create a smart component.

We begin a smart component by choosing the pulldown menu TOOLS>MAKE SMART COMPONENT.

Figure 28. Tools > Make Smart Component.

We will then be asked to choose the component which is the “smart component.” We will choose the 3 Prong POWER Port as shown in Figure 29.

We will also be asked to choose any additional components to be included with the smart component, and these components will automatically be positioned whenever we use and reuse the smart component. For our assembly, we will choose the screws and nuts (mounting hardware), as shown in Figure 29.

Lastly, we will be asked to select any in-context features which should be recreated whenever we use and reuse our smart component. For our example we will choose the in-context cut extrude representing the holes for the POWER port and the mounting hardware, as shown in Figure 29.

Figure 29. Selecting elements of smart component.

We finish by hitting the green checkmark and saving the assembly. After saving the assembly we see that the 3 Prong POWER Port displays in the tree with a little lightning bolt on the part icon.

Figure 30. Smart component indicator in the assembly tree.

This lightning bolt tells us that we have successfully created a smart component from the 3 Prong POWER Port. We can now save and close the current assembly.

Testing the Smart Component

At this point, we will create a new “Test Assembly” to ensure that the smart component is working as desired. We will begin by creating a simple L-shaped part, using the dimensions shown in Figure 30. After creating this test part, we will add it to an assembly and save the assembly as “Test Assembly 1.sldasm.”

Figure 31. Our “test component” in our “test assembly.”

Next, we will insert two instances of the “3 Prong POWER Port” on the two faces of our test part. We should mate these parts into place on the faces of our “Test Component.” We can also add distance mates from the edges.

Figure 32. Add two instances of the 3 Prong POWER Port to the assembly and mate them into place.

You will notice in the assembly tree that each of the instances of the 3 Prong POWER Port have the little lightning bolt on the part icon. This indicates that these parts are “smart components.” We can click the RIGHT MOUSE BUTTON on these components and choose “INSERT SMART FEATURES.”

Figure 33. Insert Smart Features.

After beginning the command, we will be asked to select two faces. These are the faces where the CUT EXTRUDE begins and where the HEX NUTS are mated. We will select the front and rear faces of the our model, as shown in Figure 34.

Figure 34. Select these two faces.

Repeat this process for both power ports. When finished you will be happy to see that the smart component added the screws and nuts and even the cut extrude to the test component, as shown in Figure 35.

Figure 35. Mounting screws, nuts, and cutouts added to test part.

Now that we have successfully added our smart component to a test environment, let’s go back to our original model of the guitar amp. We will add the smart component of the 3 Prong POWER port to the rear panel of the amp and mate it into place.

Figure 36. Rear panel of the amp before adding the power port.

Figure 37. Rear panel of the amp after adding the power port and mating it into place.

And now we are ready to click the RIGHT MOUSE BUTTON and INSERT SMART FEATURES. We will follow the same steps as the test assembly and select the front and back faces of the rear panel of the amp.

Figure 38. Rear panel of the amp after using INSERT SMART FEATURES.

And now the holes have been cut into the rear panel part, and the mounting screws and nuts have been added to the assembly and mated to the appropriate faces.


Learning how to leverage Design Library Features and Smart Components can be one of the greatest time-savers found in the SOLIDWORKS software. Design library works great when using one or more features and wishing to drag and drop this set of features onto multiple part files. In our example, we used a common feature (a pattern of venting slots) found on several models of guitar amps.

A Smart Component can similarly use and reuse features, but can also incorporate part files to be automatically positioned when dragging and dropping the smart component. In our example, we applied “Smart Features” to a three-prong power port so that, whenever we drag and drop this part onto the back panel of a guitar amp, we can automate the creation of the required cut extrude features as well as automate the insertion and positioning of the required screws and nuts to mount this part on our amp. This will prove to be a huge time-saver since we use power for all of our amps.

About the Author

Toby Schnaars is a Certified SOLIDWORKS Expert from Philadelphia, PA. He has been working with SOLIDWORKS software since 1998 and has been providing training, technical support and tips and tricks since 2001.

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