# How to Define a Shaft Using SOLIDWORKS MBD

We shared hole callout tips and tricks at length in the previous three articles: part 1, part 2 and part 3. However, we can’t leave out shafts when talking about holes, because holes are often designed to support shafts. In this article we’ll explore some key SOLIDWORKS MBD techniques by defining a typical shaft in a gearbox to transmit torques and rotation.

There is another reason to take on shafts. A designer once asked me how to dimension to the tangential or silhouette edges on resolved features such as cylinders and cones. These features are easy to define in 2D drawings because they are projected down to a 2D plane. In 3D, the intersections between a model and a projection plane provide profile edges to dimension to, but these edges are conceptual and imaginary. They don’t actually exist on smooth revolved features. Shafts are primarily constructed of revolved cylinders and cones, so defining them in 3D requires a different approach from 2D drawings.

Let’s start with the chamfer in Figure 1 as an example. In 2D drawings, we would just pick an edge, or the intersection between the chamfer and the 2D projection plane, and then call out the dimensions and tolerances. Here in the model-based approach, as discussed in a previous article, “Design for Manufacturing: How to Define Features Directly,” DimXpert focuses on manufacturing features rather than edges. So we just need to click on the chamfer face and it’s automatically recognized as a chamfer. Then the relevant parameters are given all together, including the length, length tolerance, angle and angle tolerance. It’s worth noting that we need to use the DimXpert Size Dimension command as opposed to the Location Dimension command, although a chamfer is not a feature of size in GD&T (Geometric Dimensioning and Tolerancing) terms. It may be more intuitive to remember it this way: We are dimensioning an overall chamfer size, rather than a location or a distance.

Figure 1. A chamfer callout on a shaft using DimXpert.

Of course, we can also recognize the shaft as a cone and the cone angle with its tolerance is pulled out automatically as shown in Figure 2.

Figure 2. A cone angle and tolerance callout on a shaft using DimXpert.

If we are happy with these two types of predefined DimXpert feature callouts, we are all set. But it may get a bit trickier when we want to customize these callouts. For example, some engineers may be asked to explicitly present half the cone angle—30 degrees—instead of the full angle—60 degrees, in the case of Figure 2—because their machinists need the half angle to lathe a chamfer.

Now it’s time to introduce another 3D dimensioning and tolerancing tool, Reference dimension, as shown in Figure 3. We can access this command by pressing the Smart Dimension button on the SOLIDWORKS MBD command bar and then picking the Reference dimension button highlighted on the left.

Figure 3. Reference dimension.

We will elaborate on the differences between DimXpert and Reference dimension later, but in a nutshell, DimXpert focuses on defining 3D manufacturing features, while Reference dimension is an extension of 2D drawing capabilities into 3D, so it may be easier to call out basic geometric elements such as lines, edges and curves. In other words, if you want to support featured-based downstream manufacturing automations, DimXpert fits better because it’s feature-oriented and its callouts are more readable by software applications. If you just want “3D drawing” annotations for human interpretations, Reference dimension can be more flexible.

Let’s explain with this shaft example. Figure 4 shows a reference dimension calling out the diameter of a circular edge. It doesn’t define the cylinder feature, but a human reader can probably infer the Φ17.5 mm as the diameter of the cylinder, too. A software application may encounter some challenges here since the unambiguous feature definition is missing.

Figure 4. A reference dimension on a circular edge.

Let’s come back to the cone feature in Figure 2. For machinists, they need the 30 degrees to set the lathing angle between the cutter and shaft axis. Figure 1 showed the approach of a predefined DimXpert manufacturing feature. Now let’s try the Reference dimension command. There are three key steps:

1. Orient the display per an annotation view. The Top view was selected as an example in Figure 5.

Figure 5. Orient the display per the Top annotation view.

2. In a Reference dimension command, click on the silhouette edge of the chamfer, which is the imaginary intersection line between the revolved face and the screen display plane. The silhouette edge selection is a key tool to solve the revolved feature challenge we mentioned at the beginning. Here we obtained the edge linear dimension as shown in Figure 6. Please don’t place it yet since we are going after the angle, not the length.

Figure 6. Click on the silhouette edge of the chamfer.

3. In the same Reference dimension command, click on the silhouette edge of the cylinder. Now we can place the 30-degree angle dimension in Figure 7. Please notice the two constructive silhouette edges are highlighted in green.

Figure 7. Click on the silhouette edge of the cylinder.

Depending on the mouse cursor location, it may also give us 150 degrees as shown in Figure 8.

Figure 8. A 150-degree callout when the mouse cursor is in the wider supplementary angle area.

The trick to locking it down is to right-click when the angle is 30 degrees. The special mouse cursor icon in Figure 7 actually gave us a hint: The blue right mouse button and the blue lock indicated the option to right-click to nail down a dimension value. In Figure 9, the angle stayed at 30 degrees even when the mouse cursor was in the supplementary angle area. This time, the icon was a bit different, indicating a right-click can unlock this value. Thus we can switch back and forth between an angle and its supplementary angle very easily.

To recap, we discussed the differences between DimXpert and Reference dimensions. Then we used a reference dimension to call out an angle by leveraging the silhouette edge selection capability. At the end, we shared a quick UI trick to lock down a dimension value. These tips and tricks are not very easy to discover, so may not be well known to many engineers. I hope you find them helpful. To learn more about how the software can help you with your MBD implementations, please visit its product page.

Oboe Wu is a SOLIDWORKS MBD product manager with 20 years of experience in engineering and software. He is an advocate of model-based enterprise (MBE) and smart manufacturing.