This is the third article in the “Do You Believe in SOLIDWORKS 2022?” series, where we dissect and put under the microscope the enhancements introduced by the latest version of the software.
Figure 1. Do you believe?
The first two articles, Fast Drawings of Slow Assemblies and Coordinate Systems Now Mightier Than Origins, Planes and Axes, established the following criteria for judging if a new enhancement is eligible for the “I Believe!” pin:
- Security. It should not introduce new bugs or regressions. If anything, the software should operate more securely than before.
- Ease of use. SOLIDWORKS users expect their software to be intuitive.
- Clear benefit. The new feature should eliminate limitations in functionality or increase productivity.
- Wide use. The more use cases in more industries, the better.
- Requested by users. Users get what they asked for.
Enhancements and… Enhancements: The Evolution of Functionality in SOLIDWORKS
I have a theory about how enhancements mature once injected into the software that can be summarized in one word: gradually.
No brand-new functionality completely satisfies all users. It usually takes several years until the functionality expands to cover more use cases, bugs are worked out, the user interface is further refined and most users are adopting it.
Figure 2. Example of the typical progress for improving a specific functionality of the software.
That makes a lot of sense, if you think about how the enhancement request and implementation process works.
Most SOLIDWORKS enhancements are born from one user’s idea for solving a personal challenge. Usually, the scope of these ideas is narrow, being focused on improving the areas of the software responsible for getting a particular job done. Once the SOLIDWORKS product definition (PD) Team gets involved, the idea gets defined and starts becoming an enhancement.
Many times, the PD team would expand the use case of a new enhancement beyond the original request; but even so, the first release of an enhancement will have a narrow scope. An example of an enhancement in its first release is the functionality added to the coordinate systems in SOLIDWORKS 2022. It is a game-changer but, as our previous article demonstrated, it has not reached even half of its potential. We hope to see more in SOLIDWORKS 2023 and beyond.
Figure 3. Enhancement stuck at 95 percent of its potential. The missing 5 percent stops users from adopting it.
Other enhancements get stalled at 95 percent of their potential, even though they seem brilliant when experienced AEs demonstrate them. After the initial release, users will try the new functionality and will find some ways the tool does not do what they need. Many times, that is also the last time the users will touch that tool. One example is the SpeedPak tool, which brings so much promise (instant simplification of the body data while preserving graphics data). Unfortunately, the missing 5 percent in its functionality soured 95 percent of the users who tried it. After that, they will never adopt it.
However, there are also those enhancements that complete the missing 5 percent in functionality for a tool, making it complete. An example is the latest enhancement for managing configurations, introduced by SOLIDWORKS 2022: the configuration table.
Building on Existing Functionality
Let’s take a quick stroll down memory lane and remember the evolution of the major tools used for creating and managing configurations using tables.
SOLIDWORKS 1997
- Excel design tables used for managing configurations. In this case, the power of Excel acts like on of Marvel’s Infinity Stones, conferring upon users superpowers for automating configurations using advanced formulas and data. Unfortunately, some users abused this power by creating design tables in all parts, even for simple configurations. When Excel and SOLIDWORKS work together, the system slowed down and was prone to crashes.
SOLIDWORKS 2010
- Ability to save configuration table views (which removed the need for Excel). This was a great tool for the regular user. The functionality worked fine for most use cases, but it was not intuitive, nor powerful enough.
SOLIDWORKS 2022
- Improved configuration table view functionality. The missing 5 percent of functionality for configuration table views was added.
- Ability to insert a configuration table in all parts or assemblies with more than one configuration. This is a great tool for the casual user. Once the system options are configured as per the instructions in this article, a very intuitive tool becomes available in all parts and assemblies.
It is interesting to note that as new tools have been added, the old ones have been preserved. Each of them has a place in the toolbox of a SOLIDWORKS power user. Many times, users would use one, two or all three options.
For example, you can have a design table to drive dimensions using complex formulae, several table views for driving subsets of dimensions/features/components/configuration properties, as well as the configuration table for quickly accessing all variables.
Figure 4. So many choices, so many use cases.
Comparing the Table Views from 2021 and 2022 for Parts
The same part was opened in SOLIDWORKS 2021 and 2022. The 2021 table view is shown in Figure 5 and the 2022 table view in Figure 6.
Figure 5. Part table view in SOLIDWORKS 2021.
Figure 6. Part table view in SOLIDWORKS 2022.
Note the two extra buttons on the bottom of Figure 6. They provide a quick way to ensure only relevant information is displayed.
Users can hide the columns related to dimensions and features (Figure 7) or the ones related to configurations parameters (Figure 8).
Figure 7. Columns driving dimensions and sketches/features suppression are hidden.
Figure 8. Configuration Parameters are hidden.
Before SOLIDWORKS 2021, the only way to customize configuration parameters was using Configuration Properties, which was a very tedious process since each configuration needed to be accessed individually. A pleasant surprise is the new option Set Exclude from bill of materials when inserted into assembly which becomes available in SOLIDWORKS 2022 (Figure 9).
Figure 9.
The user is still required to name each table view and press the save button to create or update one.
Comparing the Table Views from 2021 and 2022 for Assemblies
The 2022 enhancements are even more substantial in the assembly environment.
The same assembly was opened in SOLIDWORKS 2021 and 2022. The 2021 table view is shown in Figure 10 and the 2022 table view in Figure 11.
Figure 10. Assembly table view, 2021.
Figure 11. Assembly table view, 2022.
In addition to the features and parameters button, notice the components button that could hide and show the component related columns.
Also, note the fixed column that could be excellent for a quick check if the optimal mating scheme has been used.
“Unconfiguring” a Dimension, Feature or Component
Many times, users would require applying the same value or suppression status for a dimension, feature, or component. That is easily done in SOLIDWORKS 2022 from the table view by right-clicking on the header and taking advantage of the unconfigure tool.
Figure 12. Unconfigure.
When Unconfigure is used, the setting from the active configuration is applied to all configurations.
The New Configuration Table
While Table Views are very useful, the user needs to remember to name and save them. Wouldn’t it be nice if a table containing all variations in a part or assembly would always be readily available?
That is now possible in SOLIDWORKS 2022. Moreover, one extra piece of functionality is reserved only for this table—the ability to block manual model edits outside this table.
Figure 13. Right-click on the header and select block model edits.
Figure 14. The column becomes pink. To allow model edits, right-click again and chose the desired option.
When you block edits, the column displays in a different color. To change this color, click Tools > Options > System Options > Colors. Modify the Dimensions, Controlled by Design Table color setting.
Figure 15.
When the user attempts to manually modify the model (in this case, trying to unsuppress the coincident relation) the error message shown in Figure 16 appears.
Figure 16.
How to Activate the New Configuration Table Functionality
If you read the What’s New in SOLIDWORKS 2022 document, you might be under the impression that is enough to open any existing part or assembly with more than one configuration, and the new Configuration Table will magically appear in the Configuration Manager.
In SOLIDWORKS 2022, you will still need a couple of steps to unlock this functionality.
Step 1: System Options > General > check the Create configuration tables on open box.
Figure 17.
If this box is not checked, there will be no configuration table when opening existing parts or assemblies.
Step 2: Open a file containing multiple configurations. Be aware that in SOLIDWORKS 2022 SP0, a configuration table will not magically appear the moment you created a second configuration in a part or assembly. You would need to save and close the file. The table will be created when it is reopened.
Note that in SOLIDWORKS 2022 SP0, double-clicking on the Configuration Table in the Configuration Manager will not open the table. You need to right-click on it and select Show Table (Figure 18).
Figure 18.
Conclusion
The enhancements in the Table View functionality, along with the new Configuration Table represent the missing 5 percent in functionality that users were expecting for a long time. We now have a powerful set of mature tools that should make creating and managing configurations a breeze.
For that, we decide to wear the I Believe pin.
Let us know if you would like more articles from the I Believe in SOLIDWORKS 2022 Series.
Learn about all the new SOLIDWORKS 2022 enhancements with the ebook SOLIDWORKS 2022 Enhancements to Streamline and Accelerate Your Entire Product Development Process.
About the Author
As an Elite AE and Senior Training and Process Consultant, working for Javelin Technologies – a Trimech company, Alin Vargatu is a Problem Hunter and Solver.
He has presented 31 times at 3DEXPERIENCE World and SOLIDWORKS World, once at SLUGME and tens of times at SWUG meetings in Canada and the United States. His blog and YouTube channel are well known in the SOLIDWORKS Community.
In recognition for his activity in the SOLIDWORKS Community, at 3DEXPERIENCE World 2021, the SWUGN (SOLIDWORKS User Group Network) awarded the SOLIDWORKS AE of the Year title to Alin Vargatu.