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Toby’s Top Tips for 2019

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Toby’s Top Tips for 2019

SOLIDWORKS 2019 SP0 was released in October of 2018, and some amazing new features were added with the release. Here is a list of some of my favorite enhancements. Although SOLIDWORKS 2019 added a lot to Visualize Renderings, Simulation, Machining and Flow Simulation, I chose to primarily stick to enhancements found in CORE SOLIDWORKS CAD for this list.

1. New TRIM option in sketch mode

Have you ever been in a sketch and wanted to do a trim, but also wanted to leave the trimmed lines behind, as construction geometry?

Figure 1. My goal is to trim this line, but I want to leave it behind as construction geometry.

In Figure 1, we can see a scenario that comes up fairly often. In 2018 we would have to perform a split command, split this line in two places, turn the middle section into construction, and then assign coincident relationships to the two endpoints. That’s a lot of work!

In SOLIDWORKS 2019, using the new trim options, we can get to the same goal with a simple swipe of the mouse.

Figure 2. The new trim option to KEEP TRIMMED ENTITIES AS CONSTRUCTION GEOMETRY.

In Figure 2, we can see the new options found in the trim command.  Once we enable the option to KEEP TRIMMED ENTITIES AS CONSTRUCTION GEOMETRY we can simply perform a power trim across the desired section of our sketch.

Figure 3. The sketch, after doing a power trim using the new 2019 option.

In Figure 3, we can see that our sketch has given us the desired results, and instead of deleting the trimmed section of the line, we have simply converted it to construction geometry. Nice!

2. Better control over Intersection Splines

For many releases, we have been able to grab the intersection of two faces to generate a spline. Let’s say we have planar surfacing running through the center of a skateboard deck, as shown in Figure 4.

Figure 4. The brown planar surface is running through the center of the skateboard deck.

We could utilize the command TOOLS>SKETCH TOOLS>INTERSECTION CURVE to grab the intersection of the surface and one (or more) of the faces of the skateboard deck.

Figure 5. The red sketch represents the INTERSECTON CURVE of the face of the skateboard and the planar surface.

In Figure 5, we can see what the intersection of the planar surface and the lower face of the skateboard might look like (shown in red).

Although we have had the ability to generate a spline using commands like INTERSECTION CURVE, CONVERT ENTITIES or OFFSET ENTITIES for many releases, it was very difficult to work with this spline after it had been generated. Even when we deleted the sketch relationships on these splines, they remained rigid and difficult to manipulate.

SOLIDWORKS 2019 solves this challenge by implementing the use of control polygons onto these converted splines. After utilizing the INTERSECTION CURVE command, we can examine the spline, and we see that it has a sketch relationship.

Figure 6. The resultant spline from the INTERSECTION CURVE command with a sketch relationship circled in red.

Next, we are going to delete this sketch relationship.

Figure 7. Select the sketch relationship and press delete.

In previous versions of SOLIDWORKS, even after deleting this relationship, the spline would remain rigid and difficult to edit.

Figure 8. Click the right mouse button on the spline and choose SHOW CONTROL POLYGONS.

 In SOLIDWORKS 2019, we can click the right mouse button on the spline and choose SHOW CONTROL POLYGONS, as shown in figure 8. This great new enhancement generates a series of grip handles we can use to modify the spline.

Figure 9. Select and drag one of these control polygon grips to manipulate the spline.

Thanks to this great new feature, resizing the spline is simply a matter of dragging and dropping these polygon grips.

3. Tab and Slot command now has “Mickey Mouse Ears”

The Tab and Slot command was added to the software in SOLIDWORKS 2018.

Figure 10. A model being setup for TAB and SLOT

With the TAB and SLOT command, we can take two bodies and, with a single command, add a series of tabs to one body and a series of slots to a second body.

Figure 11. The same model, after adding the TAB and SLOT command.

This command is a huge time saver for users who are working a lot with manufactured parts that need to be fitted together for welding, as they can now fit these parts together without the need for a fixture.

However, many users were asking for additional options in the corners of the SLOTS, and SOLIDWORKS 2019 delivers these options!

Figure 12. New options for the slot corners in a TAB and SLOT command.

In SOLIDWORKS 2019, users can now choose to utilize sharp corners, rounded corners, or chamfered corners in the slots.

Figure 13. The slot with the “Slot Circular Corner” option.

Or users could chose my favorite option – the “Slot Circular Corner” option—which is sometimes referred to as “Mickey Mouse Ears” in the manufacturing world.  J

4. Partial Chamfer/Fillet

One of the most requested enhancements to the SOLIDWORKS software has been added in SOLIDWORKS 2019. Typically when we create a chamfer or fillet, we have to utilize the entire edge of a model.

Figure 14. Adding a chamfer to a model and needing to select the entire edge of the model.

SOLIDWORKS 2019 has introduced the new option for PARTIAL FILLET or PARTIAL CHAMFER edge selection.

Figure 15.  The fillet/chamfer options for Partial Edge Parameters

By using this option, users can now either enter an offset value or simply drag and drop a note to define the start and end location for their chamfer or fillet.

Figure 16. Choosing to only to add a chamfer to a section of the edge, rather than to the entire edge.

This amazing enhancement can save users lots of time. In previous versions of the software, a common workaround to accomplish a partial chamfer was to either create a complex sweep cut, or to split the model into two bodies and perform the chamfer on only one of the bodies, then re-combine the bodies back together. SOLIDWORKS 2019 can save users a lot of work with this great new partial chamfer/fillet option.

5. Multi-Body Part Interference

SOLIDWORKS has had assembly interference detection for a long time, and several years ago SOLIDWORKS added options to detect interference between bodies within a multi-body part within an assembly. This means that if you have a multi-body part in your assembly, you could check interference between the bodies of this part file. However, you could only do this in an assembly mode. This means that, if you’re like me and you do a lot of multi-body part design, and you want to check interferences between the bodies of your one single part file, you still had to take a moment and add this one single multi-body part to an assembly. Then, and only then, you could run an interference detection.

Figure 17. A single part file with multiple bodies, and the interference detection command showing on the Evaluate toolbar.

I am happy to announce that, in SOLIDWORKS 2019, we can save time by jumping right into the interference detection command while in part mode. As you can see in Figure 17, we are working in part mode on a multi-body part, and the Interference Detection tool is available on the Evaluate toolbar.

Figure 18.  A single part file with multiple bodies, and the interference detection results.

This is a nice little gem in 2019, and it saves us that extra little step of needing to create a new assembly.

6. Save Animations directly to MP4

Another little gem in SOLIDWORKS 2019, but one that I really appreciate, is the ability to create an animation and save it in some new file formats, including .MP4, .MKV and .FLV.

Figure 19. New file types available for animation output.

I love making animations in SOLIDWORKS, but this often involves a time-consuming additional step of post=processing the output AVI into a more universal format like MP4. With the new enhancement, I can skip this post-processing step. SOLIDWORKS 2019 makes it much easier to take my output animations and share them immediately with my customers.

7. New tools for working with Exploded Views

SOLIDWORKS 2019 has added some cool new functionality to the Exploded View command.

Figure 20. An exploded view in SOLIDWORKS 2019.

First, in Figure 21, we see that, when examining an exploded view in the Configuration Manager of SOLIDWORKS 2019, we now have a new Rollback Bar.

Figure 21. The new Rollback Bar in the Configuration Manager of SOLIDWORKS 2019.

Using this rollback bar, we can roll backwards and forwards through the steps of an exploded view. This is a great way to convey ideas to the team, during a design review meeting.

Next, we’ll take a look at the exploded view property manager by doing a right mouse button on the exploded view and choosing EDIT FEATURE.

Figure 22. The step forward and step backwards button in the exploded view property manager.

As we can see in Figure 22, we also have the rollback bar in the exploded view property manager, but we also have two new buttons which allow us to STEP FORWARD or STEP BACKWARDS in the exploded view process.

Figure 23. We press the STEP FORWARD button a few times to go down to Explode Step5.

In Figure 23, we can see that the rollback bar is between Explode Step5 and Explode Step6.  Another enhancement to SOLIDWORKS 2019 can be seen when we need to inject a new exploded view step here. We can simply roll the bar between Step5 and Step6, and then add our new exploded view step by dragging and dropping components in the graphics area.

Figure 24. Injecting a new exploded step between two existing steps.

The new options added to SOLIDWORKS 2019 facilitate a much more intuitive workflow when creating and modifying exploded views.

8.  Edrawings Free now has the Measure command

SolidWorks has made the excellent announcement that all of the functionality previously found in Edrawings Professional 2018 has been migrated into the free version of Edrawings 2019.

Figure 25. Edrawings Free now includes the Measure command.

In previous versions of Edrawings, the measure command was only available to Edrawings Professional users. I’m happy to see that the measure tool is now available for all files, and for all versions of Edrawings (even the free Edrawings viewer).

9.  Drawings has added the Open Progress dialog box

One of my favorite enhancements to SOLIDWORKS 2018 was the new Open Progress dialog box found in assemblies. This terrific feedback let you know how long the assembly was taking to open, which parts the assembly was accessing during open, and how long the assembly took to open during the previous session.

Figure 26. The Open Progress dialog box for a drawing.

This is all important and useful feedback, and as we can see in Figure 26, SOLIDWORKS 2019 has added this great functionality to drawings, so that we can see this same great feedback whenever we open a larger drawing file.

10. Enhanced Graphics Performance

And my final (and most significant) enhancement to SOLIDWORKS 2019 has to be the addition of the new ENHANCED GRAPHICS PERFORMANCE option.

Figure 27. The option for Enhanced Graphics Performance in SOLIDWORKS 2019

This option is truly revolutionary in the sense that it can make assemblies perform 5x, 10x, 20x or even greater than they did in SOLIDWORKS 2018.  The reason for this amazing boost to performance has been detailed in previous articles on engineering.com including:

20 to 30 Times faster Graphics response with SOLIDWORKS 2019’s New Graphics Engine

Graphics Cards for the Latest CAD Release

So, I will simply say this: If you have a card that supports this functionality, and you work with larger assemblies, you should defiantly give this option a try.  I have, and I am already seeing amazing improvements.

Conclusion

SOLIDWORKS 2019 continues to deliver jaw dropping enhancements to the software.  This list is only 10 of the hundreds of great enhancements added to this release, and you can read all about some of the other enhancements by booting up the SOLIDWORKS 2019 software and choosing Help>What’s New> PDF.


About the Author

Toby Schnaars is a Certified SOLIDWORKS Expert from Philadelphia, PA. He has been working with SOLIDWORKS software since 1998 and has been providing training, technical support and tips and tricks since 2001.

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