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Fast Drawings of Slow Assemblies

CAD PDM

Fast Drawings of Slow Assemblies

For SOLIDWORKS users, October marks the beginning of the holiday season. This is the time of the year when users are invited by their VAR (value added reseller) to attend parties where they unwrap the enhancements in the latest version of SOLIDWORKS.

Watching the elves, a.k.a. the VARs’ elite AEs, unwrap each gift seems magical—and in a sense, it is. They choose the perfect use case for each new feature and know where and how to click to make it look effortless. There is never any lag or crashes in such masterful demonstrations. Their enthusiasm is contagious and most users leave the event convinced they must upgrade to the new version immediately—if not sooner.

It is most enjoyable watching the faces of the SOLIDWORKS power users in the audience. Here are engineers and designers not easily impressed by canned demos. They are conflicted; on one hand, they want to believe in the promise of the gifts unwrapped by Santa’s elves. On the other hand, they are skeptical by nature and would like to see further proof that the enhancements will be useful.

Figure 1. Do you believe?

To get the power-user stamp of approval, an enhancement must meet these minimal requirements:

  • 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. Ideally both!
  • Wide use. The more use cases in more industries, the better.
  • Requested by users. Users get what they asked for.

In a series of articles, we will select from the enhancements introduced by SOLIDWORKS 2022 that meet the above criteria. We will unwrap each carefully and will analyze each aspect of the chosen enhancement in detail.

At the end of each article, we will conclude if the gift warrants a “I Believe” or “I Don’t Believe” pin.

The Enhanced Detailing Mode in SOLIDWORKS 2022

For this article, we chose the enhancement that most closely aligns with all five criteria.

Background

SOLIDWORKS allows users to build huge assemblies. Think plant layouts, observatories, mining and forestry machines, full assembly lines and other virtual models with tens of thousands of components. If working with huge assemblies can be a daunting task, producing parametric 2D drawings based on these assemblies is an order of magnitude harder.

Think about all the relations between a line on the drawing and the edge (or even more extreme, the silhouette edge) of the model. For detailing tasks, that line must know a ton of information and make it quickly available to the user. Examples include, but are not limited to:

  • Edge ID
  • Is the edge visible or obscured?
  • Faces intersecting on that edge IDs
  • Vertices IDs
  • Part ID
  • All Nested Subassemblies IDs
  • Component color
  • Is the component visible or hidden?
  • Is the component an envelope?
  • BOM related data. At the minimum, Item number and Quantity
  • If the edge is circular, we need to know the hole callout

Historically, these were made possible by having the assembly open at the same time as the drawing. When the user would attach a balloon, a note or a dimension to the edge, SOLIDWORKS would get the required data from the assembly and display it on the drawing.

The larger the assembly, the slower this interrogation process becomes. The solution to the problem was very simple in theory: simply inject all that information in the drawing file, to allow it to open on its own, without the assembly.

If you want to learn more about how power-users, AEs, SOLIDWORKS Tech Support and the SOLIDWORKS R&D Teams partnered to define and implement the functionality for the Detailing mode, read this article: A Potential Game Changer: No More Pain Detailing Large Drawings.

Figure 2. The Detailing mode was an idea submitted by users and voted by the SOLIDWORKS Community.

Detailing Mode in SOLIDWORKS 2020

The first release when Detailing mode became available was SOLIDWORKS 2020. The functionality was revolutionary, but limited to the most popular detailing tasks (mainly applying dimensions).

Figure 3. Detailing mode functionality in SOLIDWORKS 2020.

One of the most frustrating limitations in 2020 was the inability to create secondary views in this mode. After all, a detail, crop or broken view should get all its information from its parent. The edges are already there, they just need to be scaled and cropped.

Fortunately, some of these limitations were removed the following year (Figure 4).

Detailing Mode in SOLIDWORKS 2021

SOLIDWORKS R&D worked hard to remove these limitations, and the first enhancements were revealed in the 2021 release.

Figure 4.  Detailing mode functionality in SOLIDWORKS 2021.

Users were now able to add secondary views and also extract more information from the edges directly from the drawing file.

Figure 5. Can add secondary views with no assembly loaded.

Unfortunately, with improved functionality, more data needed to be written in the drawing file. If the drawing data was not optimized for this use, the saving operation took much longer than expected (hours versus seconds).

As Mark Johnson, the SOLIDWORKS User Success Engineering Director explained:

The way Detailing mode works is every edge is assigned a unique silhouette edgeID by SOLIDWORKS behind the scenes.  High Quality Hidden Lines Removed (HLR) drawing views already have these edge IDs, so drawings save performance for HLR drawings is the same in 2020/2021 and older versions.

These unique silhouette edgeIDs are not present for Shaded or Shaded with Edges.  As a result, upon save, these edgeIDs must be generated and assigned to all shaded with edges views across all sheets.

The result is the potential for a much slower save of an SLDDRW in 2020/2021 vs 2019 and older.

Figure 6.

In summary, if a drawing view could not be set as a high-quality view, the information related to model edges could not be efficiently written in the drawing file. That makes sense considering that in draft quality views the edges are computed based on the graphics-triangles extracted by tessellating the mathematical body data of the model. Imagine the sheer number of tiny triangles edges that must be stored for each single edge.

It is worth noting that if your drawings illustrate components with imported geometry errors, the drawing views will always be draft quality and the saving operation will suffer.

The problem was discovered very late and SOLIDWORKS R&D came up with a drastic solution: a System Setting that would enable users to decide if the data required for the Detailing mode will be saved or not in the drawing file.

Figure 7. This drastic decision will impact all drawings saved on this machine.

The solution was not ideal for many reasons:

  • It applies to all drawings on that system, regardless of whether they are small or large, or if they have high quality or draft quality views.
  • It could impact the consistency of the drawing files in a company. Imagine if one user has the setting checked and another unchecked. When the first user saves the drawing, the detailing data is saved. When the second user opens and saves the drawing, the data is scrubbed, or vice versa.

Again, the partnership between SOLIDWORKS Power users and the SOLIDWORKS Product Definition Team has borne fruit. You can read more about the 10 Life-Changing Enhancement Ideas for SOLIDWORKS Users submitted to the Top 10 3DEXPERIENCE World 2021 Idea list in this article.

The above idea detailed the solution further. Quoting from the same article:

How to implement it:

This option should be a document level setting, allowing the user to decide whether to save the drawing with the Detailing data included or not.

To simplify the workflow, the Save dialog can also have a checkbox called Detailing Data to allow the user to make such decisions.

It might even be worth considering having a Large Drawing mode, similar to the Large Assembly mode, where the software can decide to save or not save Detailing data based on the rules related to the number of drawing views set to Shaded or Shaded with Edges, or related to other factors known to slow down the detailing process.

How else could the Detailing mode be improved? Turns out that trained users of large assemblies learned how to take advantage of the very efficient tools available in the Large Design Review mode to perform a large number of task involving huge assemblies. It is very easy to open a top-level assembly in seconds in order to access one or more of its subassemblies. Wouldn’t be great to be able to open the drawing of such a subassembly in Detailing mode directly from a Large Design Review window?

This is exactly what the SOLIDWORKS Community voted as the fourth idea in the 3DEXPERIENCE WORLD 2021 Top Ten List. It is interesting to note that 40 percent of the top 10 ideas were about enhancing large assemblies and drawings functionality.

Figure 8. Ideas related to Large Assemblies and Drawings are highlighted.

The other major limitation was related to the file version. Drawings saved in older versions could not be opened in Detailing mode in SOLIDWORKS 2020.

SOLIDWORKS’ Product Definition team proved one more time how much they are attuned to users’ desires, because they delivered on these ideas and more in SOLIDWORKS 2022.

Detailing Mode in SOLIDWORKS 2022

Security

Regarding security, saving Detailing mode data is now a Document Setting (figure 9).

Figure 9. Detailing mode data in SOLIDWORKS 2022.

This makes so much more sense. The users could now decide if a drawing is large enough to warrant saving the extra data required by the Detailing mode. Even more, Drawing Templates can now be used to start small drawings with the setting unchecked and large drawings with the setting check.

This is a game changer.

The decision users must make is a balancing act between file size and the opening speed. As long as the drawings are opened from fast solid-state drives (SSD), the file size is not that important, as the results of the following case study shows.

The test drawing in this exercise (Figure 10) is at the borderline for a large drawing, making it a perfect case study for this dilemma.

Figure 10.

As shown in Figure 11, there are 12 sheets, 81 visible drawing views out of which 20 are Section Views and Breakout Section Views. All drawing views are set to high quality.

Figure 11. Drawing statistics (performance evaluation).

After saving two versions of the drawing, one with the Save Detailing Data option checked and the other one unchecked, we compared the file size and the opening time in Resolved, Lightweight and Detailing modes.

Figure 12. Speed beats size!

The results are very interesting. The data required by the Detailing mode seems to take 57 percent of the file size, but SOLIDWORKS uses it to open the drawing nine times faster. In this case, the trade-off is worth making.

The other important thing for users is the performance when working with the file after the drawing is opened. Because the edges of a drawing that has Detailing mode data contain so much more information about the assembly, we noticed that the operating speed is much faster for such a drawing, even when is opened in Resolved mode. Things like dimensioning, ballooning and switching between sheets are done fast and with no lag, even if the drawing is huge and the assembly is opened in the background. When the drawing does not have this data saved in the file, there is much more lag in operation. When clicking on an edge, the software might need to ask the assembly for extra information, thus the delay.

For small parts and assemblies that take seconds to open in Resolved mode, there is no point in saving the Detailing mode data.

Improved Ease of Use

SOLIDWORKS 2022 introduced three other major enhancements related to the Detailing mode. One of them was voted for by users, as mentioned earlier in this article. The others came as a complete surprise to all of us:

  • Ability to open in Detailing mode a drawing of the top-level assembly or one of its subassemblies when the top-level assembly is opened in Large Design Review mode.
  • Ability to open in Detailing mode all drawings, regardless of their version.
  • Ability to have standard views available from dragging from the View Palette to the drawing in Detailing mode.

Let’s examine these three enhancements.

Open Drawings in Detailing Mode from Assemblies Opened in Large Design Review Mode

Opening huge assemblies in Large Design Review mode is very fast. In SOLIDWORKS 2022, when the top-level assembly or a subassembly is selected in the FeatureManager tree with the right mouse button, a new icon becomes available: Open Drawing in Detailing mode.

Figure 13. Another productivity enhancer.

This is great for users who want to use the top-level assembly as a visual directory for finding any information. With this tool assemblies can be located fast, and their drawings opened quickly.

Note that we experienced the following limitations with this tool in the Pre-Release 1 version of SOLIDWORKS 2022:

  • Could not find the Open in Detailing mode icon on the Left Mouse button context toolbar.
  • Could not find the Open in Detailing mode icon when clicking (right or left mouse buttons) in the Graphics area (Figure 14).

Figure 14.

  • Could not bulk-select multiple subassemblies in order to open all of their drawings simultaneously in Detailing mode. If you need this functionality, there are currently free add-ins available for download.

Figure 15. Cannot open multiple drawings.

Ability to Open All Drawings in Detailing Mode, Regardless of their Version

We tested this enhancement by opening a drawing saved in 2021, using Detailing mode 2022. The drawing opened almost instantaneously, but we received a warning that some functionality will not be available.

Figure 16. Limited functionality for Old File Versions.

That being said, the main detailing functions are readily available:

  • Move/Hide/Delete/Align existing Drawing Views
  • Add/Edit/Delete Dimensions
  • Add/Edit/Delete Balloons
  • Add/Edit/Delete Notes
  • Insert General Tables
  • Add/Edit/Delete Weld Symbols
  • Add/Edit/Delete Surface Finish Symbols
  • Add/Edit/Delete GTOL Symbols
  • Insert Blocks

An unexpected limitation is the impossibility to add/edit/delete markups.

Ability to Drag Standard Views from the View Palette to the Drawing in Detailing Mode

This enhancement came as a surprise. Until now, if a user required the insertion of a model view, the assembly had to be loaded. In SOLIDWORKS 2022, standard views can be pre-emptively saved in the drawing file.

To do that, several steps need to be followed.

  1. Create a new drawing.
  2. Check the Include standard views in View Palette box inside Document Properties/Performance.

Figure 17. A new document setting.

  1. In the View Palette, browse to the model that will be used by the drawing.

Figure 18. The View Palette needs to be populated.

  1. Save the drawing.

To test the results, follow these steps:

  1. Open the previously saved drawing in Detailing mode.
  2. The standard views are visible in the View Palette.

Figure 19. The standard views are now available in Detailing mode.

Note: Compare the number of views shown in Figures 18 and 19. Notice how in Detailing mode only the standard views are saved.

  1. Drag views from the View Palette to the drawing to create new model views. Be aware that you would not be able to add Projected or Section views.

Figure 20. Fast creation of Model Views.

From here, let’s add a detail view, a crop view and break the Right model view.

Figure 21. Secondary views.

Adding dimensions, notes, hole callouts, revision tables and even balloons is straightforward.

Figure 22.

We were pleasantly surprised to notice that the drawing edges are storing even the item number associated to the component.

Comparing the file size of the drawings shown in Figure 19 and Figure 22, we notice that the standard drawing views take 70 percent of the final drawing size.

Figure 23.

Additionally, a handy thing to notice in SOLIDWORKS 2022 is that Hole Tables can also be inserted in Detailing mode.

Figure 24.

Conclusion

It is clear that SOLIDWORKS continues the ambitious project it started in 2019 for significantly improving the performance of large drawings. The Detailing mode completely replaced the QuickView mode in 2022 and it is quickly borrowing more and more functionality from the Resolved mode.

This article discovered several minor limitations in functionality. Some of them could be fixed in one of the upcoming service packs. Others should be added on the list of enhancements planned for SOLIDWORKS 2023.

After extensively testing the new Detailing mode enhancements, we decided to wear the I Believe pin.

Let us know if you would like other articles from the I Believe in SOLIDWORKS 2022 Series.


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.

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