How to Build Assemblies Faster

Users who spend a lot of time building assemblies will be happy to know about some of the great new tools that have been added to SOLIDWORKS 2019. The new Assembly Bounding Box feature, Auto-Lock Hardware Rotation, and Circular Pattern Enhancements are just a few of the great new features that have been added to the most recent release of SOLIDWORKS.

New Bounding Box Tools

SOLIDWORKS 2018 added a handy new feature that allowed users to create a bounding box around a single part. This bounding box would dynamically update so that it always calculated the minimum rectangular prism into which a part could fit. 

In SOLIDWORKS 2019, this functionality has been expanded to enable users to create a bounding box around assemblies and subassemblies. The Bounding Box command can be found under the menu INSERT>REFERENCE GEOMETRY>BOUNDING BOX as shown in Figure 1.

Figure 1. Bounding Box on an assembly in SOLIDWORKS 2019.

When creating a bounding box for an assembly, you will see a property manager that is similar to the one you use when you are creating a bounding box for a single part. You will also see some new options, such as whether the bounding box should include hidden components, envelope components, or surface bodies, as shown in Figure 1.

Once the bounding box has been added to the assembly, you will see that four new fields have been added to the custom properties of the assembly as shown in Figure 2. 

Figure 2. Four new fields have been added to the custom properties of the assembly after a bounding box has been added.

These custom properties can be used for things like annotations and notes, and can also be shown on a drawing title block. Since these notes dynamically update, this can be a great way to keep track of the overall size of the assembly.

Figure 3. The bounding boxes of different level components in an assembly.

Bounding boxes can exist at the part level, the subassembly level, or the top level of an assembly. As you can see in Figure 3, each of these levels will utilize a different color to represent the bounding box.

One of the nicest elements of utilizing a bounding box is the ease with which you can add dimensions to a drawing, representing the overall size of your assembly (see Figure 4).

Figure 4. Using the bounding box in a drawing to show overall dimensions of an assembly.

As you can see in Figure 4, you can easily select and dimension the overall size of this assembly, without needing to struggle through the process of selecting the desired points, edges or faces of the model. Selecting the lines from the bounding box makes this task simple and straightforward. 

Auto-Lock Rotation Mate for Toolbox Parts

Our example assembly is looking pretty good, but we need to add a few hex bolts and washers as shown in Figure 5.

Figure 5. Our assembly is missing a few hex bolts and washers.

A common workflow to follow in this scenario involves the following:

1. Turn on SOLIDWORKS Toolbox Add-In.

2. Drag and drop the washer into the desired location.

Note that the washer is positioned but is still constrained (since it can rotate) as shown in Figure 6.

Figure 6. The washers are constrained, and the concentric mates are not locked.

After the washers were dragged into our assembly from the Toolbox Library, they were positioned in the desired location, but each washer is still free to rotate. You can see the result of this in Figure 6, where the parts named “flat washer type a narrow_ai” are shown in the tree with a minus(-) sign next to them. You can also see that the concentric mate is not utilizing the option for “Lock Rotation,” since the icon next to the mate (the double circle icon) is not filled in solid. 

Normally at this point in the process, if you wanted to fully constrain the washers, you would have to find the concentric mate related to the washer and right-click your mouse on this mate to choose Lockrotation. Doing so will fill in the circle icon solid and will fully constrain the washer. 

The team at SOLIDOWORKS recognized that users were performing this same step—over and over again—every time they added new Toolbox hardware to their assemblies. To help users save time, SOLIDWORKS 2019 has a new option to eliminate this step, by allowing users to automatically lock the rotation of newly inserted Toolbox components as shown in Figure 7.

Figure 7. The new option for “Lock rotation of new concentric mates to Toolbox components” is found in System Options.

You can start this process by going into your System Options and selecting the category for Hole Wizard/Toolbox as shown in Figure 7. You can then select the checkbox for “Lock rotation of new concentric mates to Toolbox components,” which is shown in the figure.

Now, let’s return to our example assembly, and this time we will add two new washers and two new hex bolts.

Figure 8. Our newly added hardware has the concentric mate locked and is now fully constrained.

After adding four new pieces of hardware (two washers and two hex bolts), the software displays the feedback shown in Figure 8. Our components in the assembly tree no longer show the minus (-) sign next to their names. This indicates that these components are fully constrained. You can also see that the four new concentric mates have the double circle icon filled in, indicating that the option for “lock rotation” has been enabled for these mates automatically, thanks to this great new option in SOLIDWORKS 2019.

Circular Pattern Enhancements

Back in SOLIDWORKS 2017, the circular feature pattern (used in parts) was updated to include some great functionality, including bidirectional circular patterns and the option to create a symmetric circular pattern from a center instance. Users who often work on assemblies will be happy to know that these same enhancements are now available for the assembly of circular patterns in SOLIDWORKS 2019.

Figure 9. Our goal is to pattern the hex bolt and washer into these four holes.

Figure 9 shows a common challenge in assembly modeling—we need to have a circular pattern of components, but we also need the pattern to go in two different directions, since our seed components are centered in the pattern. In previous versions of SOLIDWORKS, this challenge would have required two separate circular pattern features. 

Figure 10. Using the option for Direction 2 to create the pattern in two directions in SOLIDWORKS 2019.

After beginning a circular component pattern in a SOLIDWORKS 2019 assembly, we now have a new option called “Direction 2” as shown in Figure 10. By selecting this option, we can create the circular component pattern of the hex bolt and washer in both directions using a single command. This is a nice time saver that will help keep our tree organized, which will make it easier to update things in the event of future changes to the project. 


Users who frequently work with assemblies will be happy to see some of the great new tools that have been added to SOLIDWORKS 2019. The ability to create a bounding box around an assembly enables users to quickly keep track of the minimum envelope an assembly will fit into. The option to automatically lock the rotation of the concentric mate created when adding a Toolbox part can save lots of time, since we often insert hundreds of Toolbox parts into a single assembly. And the new assembly circular pattern option that enables users to create a pattern in two directions will save users time because they no longer need to have an additional circular pattern feature in the tree.

Once you get SOLIDWORKS 2019 installed, be sure to check out the HELP>WHATS NEW menu to see all the great new enhancements in the software. 

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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