How to Dimension Silhouette Edges Using SOLIDWORKS MBD

We introduced reference dimensions in a previous article on how to define a shaft. An important flexibility of reference dimensions is being able to select the silhouette edges of revolved features such as cylinders, cones and tori, which are frequently used on shafts. In this article, let’s dive into these detailed examples.


Cylinders are quite easy to define using reference dimensions. For the diameter, we can just pick a cylindrical face and the diameter will be given as shown in Figure 1. We can also pick a circular edge on this cylinder to obtain its diameter as discussed in the previous article. The former approach to defining a cylinder feature is recommended for easier downstream intelligent manufacturing software consumption. The latter may suffice for human interpretation.

By the way, here are several logistical reminders. The default color of reference dimensions is gray, which is distinguished from the default dark green color of DimXpert. In this article, we also will focus on dimensions and follow the general tolerances. So in the callouts, we won’t explicitly attach tolerances. If needed, we can assign specific tolerances on a callout property manager very easily. Lastly, the shaft example used here has been intentionally simplified to remove proprietary information.

Figure 1. The diameter of a cylinder using a reference dimension.

For cylinder length, the silhouette edge selection can be pretty handy using reference dimensions. With the example shown in Figure 2, which has the orientation of an annotation view, we can just click once on the silhouette edge to get the length dimension, rather than clicking twice on both ends to get the same length in the example shown in Figure 3. A limitation with the edge selection technique shown in Figure 2 is that using the cross-highlighting from a callout to its associated silhouette edge doesn’t work because this type of edge doesn’t exist. Such edges are an imaginary concept, not actual geometry.

Figure 2. A cylinder length on a silhouette edge obtained using a reference dimension (without cross-highlighting).

Figure 3. The same cylinder length determined by selecting both end circles using a reference dimension (with cross-highlighting).

Similarly, we can define all the shaft segment lengths shown in Figure 4. Please note that the highlighted overall length of 135 mm must be determined by selecting both ends (faces or circular edges) since there is no single continuous silhouette edge to give us this length.

Figure 4. The dimensions of a shaft segment length.

As you may have noticed, reference dimensions accept both a single-selection input and multiple-selection inputs. That is, when we select one entity, either a feature, a circle or a silhouette edge, a reference dimension provides the most logical callout in this context to the mouse cursor waiting for the final placement or another input to fine-tune the context. If we select another entity, the software will provide an improved callout in the new context.

Let’s work on the height of a shaft shoulder and the depth of a relief groove as more examples of multiple-selection inputs, which are also important use cases of silhouette edges. We can pick the outer profile edges of two cylinders to obtain the height or the depth, which are 8.80 mm and 0.25 mm, respectively, in Figure 5.

Figure 5. The height of a shaft shoulder and the depth of a relief groove.

As a comparison, DimXpert would experience some difficulties here because if we picked two cylinder features, the software would try to determine the distance between their center axes, which would be zero in this shaft since all the cylinders are coaxial. Therefore, DimXpert wouldn’t return anything.


Chamfers are one type of cone. We illustrated a chamfer angle and touched upon its edge length in a previous article. It’s pretty straightforward once we understand the silhouette edge selections. One point worth noting is that we can switch between three different edge length values or lock down one before a final placement with a right-click as indicated in the special mouse cursor icon shown in Figure 6. Other types of cones can be defined in a similar fashion.

Figure 6. Three values of a chamfer edge length (From left: nominal, axial
and radial lengths).


Tori are often used for shaft relief grooves, seal grooves or fillets. DimXpert doesn’t have this manufacturing feature in its library yet, so using reference dimensions to silhouette edges can help out nicely here. Figure 7 highlights R1 mm as the relief groove radius and R0.20 mm as the fillet radius. Of course, this technique can be applied to both external and internal tori.

Figure 7. A shaft relief groove radius and a fillet radius using reference dimensions to silhouette edges.

Many designers and engineers have asked how they can determine dimensions using the tangential or profile edges of revolved features with SOLIDWORKS MBD. In this article, we illustrated three examples—cylinders, cones and tori. I hope it’s helpful. The key is to orient the display according to an annotation view and then click on the tangential edges. The click location must be very accurate. Otherwise, the reference dimension may accidently pick up a parent feature. By the way, the annotation view doesn’t have to be an orthogonal one. Figure 8 shows a segment length on a silhouette edge in an isometric view.

To learn more about how the software can help you with your SOLIDWORKS MBD implementations, please visit its product page.

Figure 8. A reference dimension on a silhouette edge in an isometric view.

About the Author

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.  

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