What’s New in SOLIDWORKS MBD 2018: Define a Pattern as a Datum Feature

Take a look at Figures 1, 2 and 3. What do these three products have in common?

Figure 1. A car wheel.

Figure 2. An electric engine starter.

Figure 3. A printed circuit board (PCB) in an oscilloscope.

You probably can guess that I’m referring to the mounting structures that are called out by the red arrows or circles in Figures 1, 2 and 3. These structures could either be the circular mounting holes on your car wheels, or the distributed holes and fasteners on a printed circuit board (PCB) in an oscilloscope or your smartphone. In order to assemble multiple parts together, mounting clearance holes are widely used in mechanical and electrical designs. Because these holes stabilize a part by removing the rotational and translational degrees of freedom, they are often established as datum features for machining and inspection.

Here comes another question for you. In the simplified designs shown in Figures 4 and 5, are the geometric dimensioning and tolerancing (GD&T) definitions the same in the two figures?

Figure 4. Define two mounting holes as two separate datum features.

Figure 5. Define a pattern of two mounting holes as one datum feature.

The models are identical in Figures 4 and 5. The difference in the two figures is that one defined two mounting holes as separate datum features B and C (Figure 4), while the other specified the hole pattern of multiple holes as one datum feature B (Figure 5). These are totally different definitions that serve different needs. Here are the differences. To mount this part, most of the time, the multiple hole instances in an entire pattern act with equal chances of contact to stabilize the structure, so both or all of the instances in a pattern should function equally and simultaneously. In other words, there is no priority of one hole over another. Therefore, it’s important to define the entire pattern, rather than individual holes, as a datum feature. The practice illustrated in Figure 4 should only be used when there is indeed a necessary ranking order among the hole instances.

The ASME Y14.5: 2009 GD&T standard shown in Figure 6 interprets the practice shown in Figure 5 further.

Figure 6. Define a pattern as a datum feature as interpreted in ASME Y14.5: 2009.

You can see that by defining the hole pattern as datum feature B, the theoretical datum axis B established by the four-pin datum simulator is actually at the center of the pattern, rather than any of the hole axes. This practice better serves the need in this instance. What matters most in this design is the accurate positioning of the plate center because it determines the positioning of two M20 threaded holes. On the other hand, the individual mounting holes at the bottom of Figure 6 really don’t matter much because they don’t carry out the core function of the design. As long as they can collaboratively locate and stabilize the overall structure, their mission is accomplished.

The car wheel shown in Figure 1 provides another example. A key requirement for a car wheel is to accurately rotate across its center. Otherwise, the car would bounce up and down while it is being driven on a road. Consequently, it’s strongly recommended that you define the entire pattern of the wheel’s five holes as a datum feature to accurately control the center position.

There are other advantages to this practice. For example, because you don’t have to define one hole as datum feature B, the next as C, the next as D, and so on, there is no tolerance accumulation. In other words, a subsequent datum feature wouldn’t have to collect or be impacted by all the tolerances from the previous datum features. As a result, the manufacturing accuracy and quality are better. Furthermore, because the key requirement is on the collaborative result of the mounting center, the tolerance on each individual hole can be loosened. For a simplified example like the one shown in Figure 5, one hole location may shift a bit to the right, but if the other hole on the other side shifts by the same amount to the right, then two gauge pins on a datum simulator can still fit into the two holes simultaneously, so the part will still be good. In this way, you can save on costs because an inspection can accept parts that would have otherwise been rejected due to individual shifts in the hole center.

Now that the real-world use cases and advantages of a pattern as a datum feature have been clarified, let’s take a look at how SOLIDWORKS MBD 2018 supports this practice. Figure 7 shows an example with one of the NIST product and manufacturing information (PMI)validation conformance test models.

Figure 7. Pick a hole pattern as a secondary datum in the Auto Dimension Scheme.

The software lets you define a model manually or automatically. In this example, I’m using the Auto Dimension Scheme. I picked the bottom face as the primary datum feature. Then, for the secondary datum feature, I clicked on one of the surrounding mounting hole edges. SOLIDWORKS then recognizes that this edge belongs to a hole that belongs to a pattern. So, the software presents several practical options, including a cylinder, a hole and a pattern, as the default selection, and a compound hole. Let’s just keep the default selection and continue to identify the target features to annotate. Next, please click on the green check mark in the auto dimensioning command, and you’re done. The workflow is pretty simple and fits nicely into the existing software functions. Figure 8 shows the results in which the four mounting holes serve together as the datum feature B, and the 10 holes on the top face are positioned to the datum reference frame established by A and B at the maximum material boundary.

Figure 8. A pattern of four holes is defined as datum feature B.

By the way, the pattern recognition and selection as a datum feature are not limited to native SOLIDWORKS models. Imported models are also supported. Figure 9 shows that you can leverage this new enhancement with an NX model.

Figure 9. Select a pattern as a datum feature from an NX model.

If you define a datum feature manually and there is an existing pattern callout to that feature, then the datum symbol will automatically jump to the callout (as shown in Figure 10) to tighten up the viewport display and comply with the ASME Y14.5: 2009 standard.

Figure 10. A datum symbol automatically jumps to an existing pattern callout in compliance with ASME Y14.5: 2009.

With that, let’s conclude this article. Patterns as datum features are widely used in products from automotive to consumer electronics. SOLIDWORKS MBD 2018 can support this practice with both manual and automatic annotations for both native and imported models.

If you have any comments or questions, please feel free to leave them in the comments area below. To learn more about how SOLIDWORKS MBD can help implement your model-based enterprises, 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 and smart manufacturing.

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