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Tips and Tricks for Defining and Organizing Hole Callouts in SOLIDWORKS MBD

CAD Concept Design

Tips and Tricks for Defining and Organizing Hole Callouts in SOLIDWORKS MBD

For mechanical engineers and designers, holes are one of the most frequently used features in engineering design. They are often used to mount other components or to support shafts. In the first part of this guide, we worked on internal and external diameters in Figure 1’s section view. Now let’s continue to define the remaining dimensions and tolerances in a way similar to 2D drawings. We will cover many other useful tips and tricks in this second article.

By the way, in model-based definition (MBD) implementations, product and manufacturing information, or PMI, is a general term that has been widely adopted. It includes dimensions, tolerances, notes, datums, geometric tolerances, weld symbols, tables and so on.

2D_DrawingFigure 1. 2D drawing of a simplified bearing housing.

First, let’s work on the four length dimensions at the bottom of the left view in Figure 1. For distances like these, we need to use the location dimension per geometric dimensioning and tolerancing standards to define feature locations rather than feature sizes. Defining the longest distance, 1.940 in, and the shortest one, 0.180 in, is easy. We can simply pick parallel planes on the model to call them out. The two in the middle are a bit tricky in that they don’t have all the necessary parallel features available on the model for us to pick. This is where intersection geometries in SOLIDWORKS MBD come in handy, as shown in Figure 2.

Figure 2. Create an intersection plane between two faces.

In the location dimension command, we can simply select one feature such as the conic face. There will be an in-context command bar with several options. Click on the “Create Intersection Plane” button on the right to select another feature to intersect with this conic face. Then pick the highlighted cylindrical face and click the green check mark. We will see an intersection plane inserted between the cylindrical face and the conic face. This inferred plane will serve as one end of the location dimension at the absence of an actual plane feature at that location. Then pick the bottom face of this bearing house on the right to get the 1.630-in callout. Similarly, we can get the 1.420-in dimension, as highlighted in Figure 3, with these steps.

Figure 3. A location dimension between an intersection plane and an existing face.

Please note the two green transparent intersection planes we just created for the 1.630-in and 1.420-in location dimensions. Once an intersection geometry is generated, we can easily reuse it for other dimensions such as the distance between these two intersection planes in Figure 3.

However, in this case, this callout may not be recommended because it would result in a closed dimension chain. If there are any tolerance conflicts in the actual machined parts, an inspector would have a hard time figuring out which tolerance is more important in this closed chain.

This point on the closed dimension chains applies to both 2D drawing and MBD. An interesting discussion topic here could be, “What 2D drawing concepts are still applicable to MBD, and by extension, which concepts are no longer relevant?” We would love to hear your feedback in the comment area below.

Besides intersection planes, SOLIDWORKS MBD can also create intersection circles, lines or points to define 3D PMI. More details can be found at this SOLIDWORKS Tech Blog post.

Now let’s finish up the left-hand view in Figure 1 by defining datum features A and B. A frequently asked question here is about the datum symbol attachment. As shown in Figure 4, the datum symbol A and the datum feature A flatness control frame are detached. Some manufacturers prefer it this way, while some may want to attach these two to make the presentation more concise. We can adjust it quickly by clicking the Gtol button on the Datum Feature property manager. When we define the datum feature B, you may notice the symbol B snaps to the hole diameter dimension line automatically. SOLIDWORKS MBD intelligently selects the dimension attachment leader style to present a concise display.

Figure 4. Adjust the datum symbol leader attachment style.

It’s time to move onto the PMI on the right-hand view in Figure 1. In drawings, multiple views are placed on a flat sheet to present the design from multiple perspectives. In MBD implementations, the view management is even more important because ultimately, MBD data needs to be presented in a consumable, actionable and professional way to guide the downstream production and to support the future sustainment. If not properly managed, piles of 3D dimensions and tolerances could look extremely overwhelming and messy. Many lessons have been learned in this regard as described in this MBD implementation article. One of the sleek view management tools that SOLIDWORKS MBD provides is called 3D Views, which can capture zooming factors, orientations, annotation views, configurations and display states all together, providing a holistic picture of your design. This blog post explains how visual, comprehensive and flexible this tool is.

In the bearing housing model, we can easily double-click the front or back 3D view to switch to the expected perspective as shown in Figure 5. We can then launch the Auto Dimension Scheme tool with the following settings: part type as Prismatic, tolerance type as Plus and Minus and pattern dimensioning as Polar. Next, we pick the bottom face as the primary datum, and the internal diameter as the secondary datum. Lastly, let’s define the scope, which is a fun piece here. We can choose to use Auto Dimension to define all features. It’s very powerful but may generate a huge amount of PMI to fully tolerance this part. For this exercise, let’s just selectively pick our target: the flange hole pattern.

Figure 5. Auto dimension a hole pattern.

The selection is really easy too: Click on a hole’s inner face (or even a hole’s edge to avoid zooming into small features), and the entire hole pattern is automatically selected. SOLIDWORKS MBD intelligently recognizes associated features and provides sensible options on the in-context command bar. As we can see, the default option is a pattern, which is what we need. There are also other options such as Cylinder, Hole, Counterbore, Create Compound Hole, Create Intersection Point and Create Intersection Plane. We can look into these in future articles.

Execute this command and we will get the polar coordinates of this hole pattern as shown in Figure 6, including the hole sizes, the circular pattern diameter and the spacing angle. You may notice the 6X in front of the hole sizes and the 60-degree angle. This instance count indicates that all six instances in this hole pattern are automatically associated and defined together. For example, if we click on the 6X 60.000°±.500° angle, all six counterbore holes will be highlighted, which complies with the ASME Y14.41-2012 standard and provides semantic intelligence for downstream manufacturing processes. Of course, if we right click on this callout, we can also choose to break this combined dimension into individual instance callouts as illustrated in the first part of this guide.

Figure 6. Polar dimensions of a hole pattern.

In this article, we covered many frequently discussed techniques, such as the intersection geometries, datum symbol attachments, 3D views, hole selection, auto dimension scheme and polar coordinates. I hope you find them helpful and practical. Your comments are welcome below. To learn more about how SOLIDWORKS MBD can help you define and organize hole callouts, please visit its product page.

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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