Ensure Solid GD&T Datum Practices with SOLIDWORKS MBD
A frequent question about 3D annotations is how a datum symbol can be attached to a centerline, an axis or a middle plane of solid bodies. This SOLIDWORKS MBD forum post provides a recent example. Datum features are the foundation of composing and interpreting geometric dimensioning and tolerancing(GD&T) definitions. When we locate a physical address on a map, we reference the country, state, city and street of the address. Datum features provide similar references in a feature control frame. So let’s look into this important topic in this article.
We can begin by asking the question: Do you see any problem with the GD&T definition in Figure 1? In the figure, datum symbol A is attached to a centerline and then is referenced in a total runout tolerance.
Figure 1. A problematic GD&T definition. (Image courtesy of a Tec-Ease GD&T tip video.)
This actually turned out to be a million-dollar problem. The original part by a customer was a lens barrel in a space telescope on which the opening at the left interfaced with a lens, which is why the total runout tolerance was controlled tightly at 0.0006 inch. Figure 1 is a simplified illustration of the part.
A tight tolerance is fine as long as the product function justifies it. The real problem with this part is the datum label attached to the centerline on the customer drawing, because it didn’t specify which tangible feature would serve as the datum feature to inspect the tight tolerance. A centerline is theoretical and intangible. In the actual production, the supplier inspector didn’t have definitive instructions on how to hold the part. Figure 2 shows an exaggerated example of a machined part by the supplier. Clearly, the smaller cylinder on the right of the figure was misaligned.
Figure 2. An exaggerated example of a machined part.
If the supplier grabs a convenient feature such as the larger outer cylinder on the left, spins the part, and then inspects the runout, the part is good as what is shown in Figure 3.
Figure 3. Inspecting the total runout by holding the convenient larger outer cylinder.
Unfortunately, the customer held the barrel in the way it would assemble in the lens mount. As a result, the smaller cylinder on the right should be spun to inspect the part based on the intent of the design. Now, as shown in Figure 4, the total runout is violated and the part should be rejected. This ambiguity led to a lawsuit of nearly$8 million.
Figure 4. Inspecting the total runout by holding the smaller outer cylinder.
This problem could have been easily avoided if the symbol was specifically defined to an intended tangible feature, rather than an ambiguous geometry. Figure 5 shows the recommended definition using SOLIDWORKS MBD. In this approach, you can select the smaller outer cylinder to define the feature. The software then highlights the actual face once a label is selected and automatically aligns the datum symbol to the size diameter and tolerance callout.
Figure 5. A recommended datum feature definition.
This lens barrel case demonstrates the costly downside of ambiguous GD&T definitions. Although this issue can occur in both 2D drawings and 3D annotations, some MBD software guides the definitions with built-in GD&T rules to ensure solid practices. For example, Johnson Controls estimated significant value benefits with improved GD&T practices in the CATIA MBD environment.
Similarly, SOLIDWORKS MBD follows the ASME Y14.5-2009 GD&T standard closely. For instance, according to this standard, the datum feature symbol B in the two figures when compared to Figure 6 conveys two completely different design requirements. The one shown on the left indicates that datum feature B is the width feature because the label B is aligned with the width dimension line, while the one shown on the right indicates that datum feature B is only a single face because the label is not aligned with the width callout.
Figure 6. A drawing comparison between a width feature as a datum feature (left) and a single face as a datum feature (right).
In order to avoid this common confusion, SOLIDWORKS MBD automatically aligns the label to the width feature size dimension line as shown on the left of Figure 7. If the design requires only a face as the datum feature, then you can define a face, rather than a width.
Figure 7. An MBD comparison between a width as a datum feature (left) and a single face as a datum feature (right).
By the way, a width datum feature gives the middle plane between the two opposing faces as the theoretical datum. I hope this answers the frequent question posed at the beginning of this article. You can find more about the differences between datum feature and datum here.
Let’s expand to several other examples. Figure 8 shows the datum features A, B and C on a shifter stick. A is the width size feature, B is the two coplanar shoulders as highlighted in green, and C is the pattern of two mounting holes that is supported by a new enhancement in SOLIDWORKSM MBD 2018.
Figure 8. Datum features A, B and C on a shifter stick.
In this ABC datum framework, I added the Maximum Material Boundary (MMB) modifiers to A and C, which are size features. This allows datum shifts to accept more good parts. However, if I were to add MMB to datum feature B as shown in Figure 9, the software would flag it because B is not a feature of size and maximum material boundary doesn’t apply in this case.
Figure 9. A warning message against using an incorrect MMB modifier.
You may also notice that when a feature control frame is selected, the coordinate system as defined by the ABC datum references is automatically created and highlighted in green in the graphics area. This provides an instant visual confirmation that makes interpretation easier. It also helps automate the coordinate system alignment for other downstream manufacturing software.
On this GD&T editing dialog, if a user forgets to type in a primary or secondary datum letter before a tertiary one in a feature control frame, the dialog automatically displays a warning message to alert the user as shown in Figure 10.
Figure 10. A warning message about missing primary or secondary datum letters.
Besides the manual annotations, the software follows the GD&T rules in the automatic dimension creation as well. Figure 11 illustrates an error in which the two datum features in the red box share the same axis. The features are defining the same theoretical datum, so the tool catches their unnecessary duplication.
Figure 11. An unnecessary datum feature duplication caught in the automatic dimension scheme.
As mentioned at the beginning of this post, when interpreting a GD&T definition, a user first needs to remember the datum references. So, a handy command is to automatically highlight the associated datum symbols and features. The 3D PDF generated by SOLIDWORKS MBD provides this command shown in Figure 12. You can right-click on a feature control frame and click on the context menu command “Highlight associated datums.” I hope that a similar handy capability can be added to the SOLIDWORKS environment in the future.
Figure 12. Highlight associated datum symbols and features for a feature control frame.
With that, let’s conclude this article with several key points:
- Datum features are the foundation of GD&T definitions.
- You should define datum features on tangible faces, rather than intangible ambiguous geometries.
- SOLIDWORKS MBD builds GD&T rules into the software to help detect violations.
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 product manager with 20 years of experience in engineering and software. He is an advocate of model-based enterprise and smart manufacturing.