Take a look at the kitchen utensil holder shown in Figure 1 and the structural steel frame shown in Figure 2. You may notice that the tabs and slots have been interlocked with each other to assemble a product.
Pairs of tabs and slots are widely used in self-locating and self-fixturing designs such as food processing machines and furniture. There is even a type of furniture specifically designed for tool-free assembly. For welded equipment, premanufactured tabs and slots can connect and stabilize multiple pieces to make the job of a welder easier and improve the welding quality.
However, the typical way to create tabs and slots is to draw a sketch to extrude a tab on one piece of paper. Then, you need to convert the entities from the first sketch to another sketch on another piece of paper to cut out a slot. After these manual steps are taken, you probably need to generate a pattern of the individual instances to make a series of tabs and slots. Following the initial creation, maintaining the association between a tab and a slot in a pair turns out to be an even more time-consuming challenge.
In fact, because of the common application and the laborious work involved, since 2007 this topic has popped up dozens of times at the SOLIDWORKS forum in the past 10 years. To speed up the steps in this process, SOLIDWORKS users have been trying different work-around, such as library features, the cavity tool or smart components, but none of them works as a designated tool. As Tom Schrei put it at the forum, “(a designated automation) would save us greatly in hours on jobs.” Finally, in SOLIDWORKS 2018, a new feature has been implemented to automatically create associative pairs of tabs and slots. Let’s take a look.
First of all, you may need to show the feature button on your command bar so that you can access it easily. You can customize the user interface by dragging and dropping the Tab and Slot button to the command bar as shown in Figure 3. Please note that the button is under the Sheet Metal category.
Now let’s start with a model as shown in Figure 4, a utensil holder that is similar to the product shown in Figure 1. Please notice that this new feature needs multi-body parts or assemblies to function properly.
Please click on the new feature button, which will then require you to provide several inputs as shown in Figure 5.
The most essential inputs you’ll need to provide are the edge for the tabs and a corresponding face for the slots. All the other parameters will be used to further fine-tune the model later. Please go ahead to pick the edge and face for the model as shown in Figure 6. You can rotate the model to select the back face. I personally find it tedious to rotate a model back and forth. So,in this case, I’m using the Select Other command to locate the back face of the model without any rotation.
Then you can see an instant preview of the creation as shown in Figure 7.
Then, please click on the green check mark on the property manager, and you will get the automatic pairs shown in Figure 8.
You may notice the two feature tree nodes on the left, one for the tabs and one for the slots. However, only the Tab tree node is editable.
Now, to verify the result, let’s check the individual bodies as shown in Figure 9. Please notice that the bosses and cuts have been added to the pieces separately.
Figure9. Patterns of tabs (left) and slots (right) are created on the corresponding bodies.
Now let’s see what kind of fine-tuning we can run. Figure 10 shows that you can offset the start and end reference points of the series. Sometimes,you may not want the series to cover the entire edge. Figure 10 shows one example of redundant pairs being improved by offsetting the start reference point and reducing the number of instances.
Figure10. Redundant tabs (left) and the adjusted result(right).
What’s sweet about this tool is that you can tweak the offsets and see the instant feedback from the yellow graphics preview. This renders the results more predictable and makes the tool easier to learn and more enjoyable to use. This type of instant display is built into multiple controls of this new feature in a way that is similar to other straightforward SOLIDWORKS functions, such as Pattern or Fillet.
For example, you can reduce the number of instances in an Equal Spacing setting, and you will see the result right away as shown in Figure 11.
Or, you can switch to defining the Spacing Length as shown in Figure 12. As you adjust the distance between two instances, the preview will update the pair locations and add new pairs as needed automatically.
By the way, the slots don’t need to be cut through. You can define the height of the cut as Blind, Up to Surface, or Offset from Surface. In this case, and as shown in Figure 13, I chose to cut by only 3 millimeters so that the other side of the slots can stay intact and look smooth.
Another useful control is the Edges Type. When you handhold two heavy welding pieces to put them together, fillets or chamfers can help guide the tabs and let them slide into the slots with less effort. The sharp edges would be really hard to fit in, especially when there are multiple pairs to match simultaneously. The edge treatments can be adjusted intuitively among Sharp Edges, Fillets and Chamfers as shown in Figure 14.
Similarly, a slot clearance between a tab and a slot can help two pieces fit together more easily. If there was zero clearance, it would be extremely tight to precisely insert all the tabs into all the slots. So, let’s give it a 0.2-millimeter clearance as shown in Figure 15.
Now you can select other edges and finish the self-locating and self-fixturing structure as shown in Figure 16.
After the initial creation, if you need to make any changes, you can simply edit the Tab and Slot feature in a way that is similar to editing patterns. All the controls that are illustrated in this article can be edited on the property manager intuitively. In other words, what you see is what you get. Furthermore, you don’t have to worry about matching a tab with its slot. It’s taken care of by the software.
I hope that you find this long-awaited enhancement relevant and helpful. If you have any comments or questions, please feel free to leave them in the comments area below. To learn more about the latest SOLIDWORKS 2018 release, please visit the product launch page.
About the Author
Oboe Wu is a SOLIDWORKS product manager with 20 years of experience in engineering and software. He is an advocate of model-based enterprise and smart manufacturing.