In a previous article, we started a quick example on how to build trust into your models in a model-centric environment. Figure 1 shows the detected issues in a prioritized order regarding the replaced dimension text, the material assignment and the annotation styles. On this list, we will examine and fix an error of replaced text in a reference dimension.
Figures 1. Prioritized issues on the Result List.
In this article, we will continue reviewing other issues and their resolutions. Besides checking reference dimensions, Design Checker also caught several DimXpert errors as shown in Figure 2.
Figures 2. Design Checker caught a DimXpert callout issue.
By the way, just in case you are wondering about the various 3D annotation tools in SOLIDWORKS, Table 1 summarizes their use cases, strengths and challenges.
Table 1. The use cases, strengths and challenges of SOLIDWORKS 3D annotation tools.
| Annotation tools | Use cases | Strengths | Challenges |
| DimXpert Dimensions | · Model-based enterprise (MBE)
· Standard compliances such as ASME Y14.41-2012, ASME Y14.5-2009, ISO 16792-2015 and ISO 1101-2012 |
· Define features semantically to automate manufacturing
· Flag Geometric Dimensioning and Tolerancing (GD&T) issues intelligently · Provide a rich manufacturing feature library |
· Don’t define geometries such as edges, lines or circles since they are not features
· May seem constrained by built-in standards and rules |
| Reference Dimensions | · 3D drawings following the traditional 2D drawing conventions | · Flexible
· Can define geometries such as edges, lines and circles · Can define a limited set of features such as holes and planes |
· Don’t include the GD&T intelligence
· Don’t provide a manufacturing feature library · Don’t have tree node representations |
| Sketch/Feature Dimensions | · Display of existing sketch/feature dimensions in 3D | · Reuse existing annotations to save efforts and maintain consistency
· Are driving dimensions |
· May cause accidental model changes by the driving dimensions
· Are not feature based · Don’t include the GD&T intelligence · Don’t provide a manufacturing feature library · Don’t have tree node representations |
Now let’s get back to Design Checker. It’s worth noting that the DimXpert issues caught by Design Checker are harder to understand than reference dimensions because they are not automatically zoomed into and the selections don’t highlight the associated features. Obviously, the software can be improved in the future, but we can trace the corresponding callouts from the result remarks shown in Figure 2.
Similar to the reference dimension issues, this type of DimXpert error is caused by manually altered dimension text, which leads to hard-coded text such as the 30X multiplier prefix shown in Figure 3, out-of-sync multipliers based upon model updates, and possibly mistaken readings made on the shop floor.
Figures 3. A hard-coded 30X multiplier prefix led to a DimXpert error.
This practice could not only result in misinformed production decisions, but also compromise the quality of machine-consumable annotations and consequently hinder the downstream manufacturing automations. Therefore, it was categorized as a critical issue that was displayed in red when we built the checking requirements.
Besides the Design Checker verifications that occur after the fact, SOLIDWORKS also pops up a warning message as shown in Figure 4 to call special attention to any manual overriding of the dimension value pointer <DIM>.
Figures 4. A warning message about overriding the dimension value text <DIM>.
Now the question is how can we fix this issue with a semantic multiplier and annotation? One way is to apply the Instance Count as designed by the software to replace the hard-coded text. Figure 5 shows the semantic annotation text on the left and the correct display on the right. Note that the Instance Count box was checked off and a string of <COUNT=#X> was inserted. Somehow in my tests, I needed to add this string <COUNT=#X> manually, which may be a software glitch. Ideally, by checking the Instance Count box, the software should take care of the text automatically so that end users don’t have to remember the syntax or manually enter anything.
Figures 5. Add an Instance Count to construct a semantic hole pattern callout.
Another way to fix the issue is to delete the fragmented problematic annotations and call out the entire countersink hole pattern together. Figure 6 shows a size dimension annotating all of the 30 instances. As a previous article noted, SOLIDWORKS provides a predefined library of manufacturing features, so that the actual manufacturability is considered and communicated accordingly. Notice that in Figure 6, the instance count, the countersink hole diameter, the countersink opening diameter, and angle, along with their tolerances, are all called out together. Of course, you may also choose to annotate an individual countersink or a simple hole. These options are available on the in-context option bar. By default, the most comprehensive option is presented, which, in this case, is the pattern as shown in Figure 6.
Figures 6. Call out the entire countersink hole pattern.
Speaking of the combined callout, there is a question on the SOLIDWORKS MBD Forum asking how to change tolerance values in a combined Size Dimension.
Because there are multiple segments in this combination, SOLIDWORKS provides a drop-down list to help you adjust tolerances for each segment as shown in the upper balloon on the left in Figure 7. Please also notice that the dimensions are all parametric and are now free of hard-coded text as pointed out by the lower balloon on the left in Figure 7.
Figures 7. Adjust tolerances by segment and notice the parametric dimensions.
Now we can move on to another category, the part document material. Figure 8 shows that there is no material specified, while the preferred material is 1060 Alloy. Thanks to this catch, you can decide to leave the material specification as is or correct this issue. It’s nice to see that automatic corrections are available for this material check. So, you can correct the selected specifications by choosing the button on the right, or choose to correct all the applicable issues by clicking the Auto Correct All button on the left. Please note that not all checks are accompanied by automatic corrections. For example, the replaced text at the top can’t be automatically fixed yet in SOLIDWORKS 2017.
Figures 8. A part document material issue and the Auto Correct buttons.
Now let’s click the Auto Correct All button to fix the material and font issues. Please compare Figures 9 and 10. Most of the issues on the Design Checker list are resolved in Figure 10. For example, the material has been changed to Aluminum Alloy 1060 and the font is now Arial Narrow instead of Century Gothic.
Figures 9. The model and potential issues before the automatic correction.
Figures 10. The model and potential issues after the automatic correction.
With that, let’s conclude this article with several takeaways:
- Design Checker can help detect issues in both 3D models and 2D drawings.
- Some issues can be automatically corrected.
- The tool shows great potential to be improved in the future, especially in 3D.
- You can build and run custom checks beyond the existing 50 or so in-product requirements. For example, the SOLIDWORKS 3D Content Central shared 15 custom checks.
Please feel free to leave your comments or questions in the comments area. To learn more about how SOLIDWORKS Design Checker can help build trust into your models, 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.