Small Changes Add up to Big Productivity
There are three major events highlighted in every SOLIDWORKS Poweruser’s calendar: the first week of February, the second of June, and the third of October.
At SOLIDWORKS World in February, users are teased with a glimpse of the new functionality that will be introduced in the next release of the software. I, for one, get so excited dreaming about the multiple ways that this new functionality could increase my productivity that I find very hard to wait until June, when the software’s Beta version becomes available for downloading and testing.
The summer is a fast and furious season, when each new enhancement is put through its paces by the users who commit to BETA testing. In the process of bug squishing, these users revisit old methodologies and “design” new and more productive techniques, incorporating the new tools into their modeling workflows.
Then October comes, and the latest release of SOLIDWORKS is released to the whole user community. The first thing users read is the What’s New document, which this year contains over 200 new enhancements.
Not all these enhancements are equal. Some of them transcend the meaning of the word enhancement, and are brand new products added to the SOLIDWORKS ecosystem, like SOLIDWORKS CAM or SOLIDWORKS Manage. Others are adding revolutionary new functionality to existing products, like the new Topology Optimization introduced in SOLIDWORKS Simulation Professional and Premium.
This article is not about these major enhancements. I decided instead to write about what some users would consider “small” enhancements, and demonstrate how seemingly small things can have a significant impact on productivity.
Without further ado, this is my top 20 new core enhancements list:
1. Bounding Box for Parts
This has been one of the most voted enhancement requests through the years, and is a must for any user who needs to list accurate, parametric finished sizes for the components of an assembly.
Almost all SOLIDWORKS users need to include the finished sizes for each part in a bill of materials (BOM). In the past, several work-arounds could be applied:
- Manually adding overall dimensions and linking them parametrically to custom properties
- Using a macro
- Defining the part as a weldment and then creating a bounding box for the cut list item
- Using the Costing add-on to create stock size custom properties
All of these work-arounds are cumbersome and time consuming. Even macros would work only for the most basic orientations and shapes, but would not update values on rebuild. There was a great need for a dedicate tool, and now we have it!
When editing a part, access the Bounding Box command from the top menu: Insert/Reference Geometry/Bounding Box. Of course, you could also add the icon to a toolbar, to your mouse gestures, to the shortcut toolbar (“S”), or to the context toolbar.
The strength of the Bounding Box tool is its ability to create a Best Fit bounding box—in essence, the smallest box in which the model could fit. Users are not limited to the best fit chosen by the system; a custom plane could also be selected as reference for the bounding box orientation.
Once the Bounding Box is created, several things occur:
- A Bounding Box feature is added in the tree. It is not history dependent, as it is located right after the Origin and the Center of the Mass features.
- A 3D Sketch of the box is added to the model. The sketch is not editable, and can only be hidden or shown.
- Four configuration-specific properties are generated automatically. They could be used in a BOM, in a title block, or as input for a concatenated property.
Let’s put the Best Fit condition to a test. I will rotate the body and see what happens with the 3D Sketch.
It looks like the new feature passed the test.
What’s next? There is a lot of potential to further enhance the functionality of this feature. We can start a list of enhancements requests with the following:
- Ability to generate bounding boxes for assemblies
- Ability to generate individual bounding boxes in bulk to all (or to preselected) components of an assembly
In conclusion, I estimate that this tool could save users 1-5 minutes per part when creating parametric custom properties. For a 1,000-component assembly, this translates to eliminating hours of boring, repetitive, intense work.
More important, the bounding boxes would update automatically when the part is modified, without any fear of losing references for the dimensions linked to custom properties, which occurred in the past. That is an even more critical benefit that the new functionality adds to the user experience.
2. STEP, IGES and ACIS Files Are Now Supported by 3D Interconnect—with Custom Properties, Too!
Working with imported geometry could be quite painful for CAD users in general, including those using SOLIDWORKS. For example, opening a STEP file in SOLDIWORKS 2017 or earlier relied on a conversion process that could take minutes or, sometimes, hours.
This whole phase can be completely sidestepped in SOLIDWORKS 2018 by taking advantage of the enhanced functionality in the 3D Interconnect tool. This enables direct read of data from STEP, IGES or ACIS files into SOLIDWORKS models, without the need to perform an actual conversion.
Moreover, SOLIDWORKS 2018 can now read reference planes, custom properties, metadata, or user-defined attributes from neutral formats and third-party native CAD files, and then map them to the custom properties of SOLIDWORKS. The supported file formats for accessing custom properties are as follows:
- Autodesk Inventor
- CATIA V5
- PTC Creo
- Solid Edge
Similar to the 2017 workflow, with SOLIDWORKS 2018 the user needs to enable 3D Interconnect default functionality from inside System Options/ Import/ General.
Now, there is brand-new page inside the System Options/ Import section dedicated to STEP, IGES and ACIS settings. Here, you can choose to import reference planes or user-defined attributes into SOLIDWORKS custom properties.
Once the neutral file is opened, a 3D Interconnect feature will be displayed in the tree, representing the link between the neutral file and the SOLIDWORKS model.
Users should be aware that the resulting custom properties are locked when the third-party CAD file and the SOLIDWORKS file are linked. To overwrite these properties, users must break the link.
There is one major limitation when the files originally from STEP, IGES or ACIS that are linked to 3D Interconnect components are revised. The face and edge IDs are not preserved when the component is relinked to a different version of the STEP, IGES or ACIS file. This means that any features or mates added to these models will have dangling references. This problem does not usually affect the traditional converted geometry.
Also, be aware that while import diagnostic can be performed on a SOLIDWORKS model linked to a third-party CAD file, any topological errors found cannot be corrected. That makes sense when you consider that we are just reading the native file inside SOLIDWORKS, not converting it.
In conclusion, in SOLIDWORKS 2018, 3D Interconnect facilitates a significant reduction in the time needed to open STEP, IGES and ACIS files (potentially saving hours), along with new functionality for importing reference planes and metadata.
3. Enhanced Perpendicular Mates
Since SOLIDWORKS 2014,when the tangent mate’s functionality was expanded to include mating between spherical faces and non-analytic geometry, the only standard mate with a major limitation has been the perpendicular mate. Something as (seemingly) simple as trying to set an edge or an axis normal to a complex surface by mating required complex workarounds.
The good news is that this problem has been resolved with SOLIDWORKS 2018. Users can now apply perpendicular mates between linear entities like a line, edge, axis or axial entity and any type of surface.
In conclusion, an apparent small enhancement could save 2-3 minutes of unnecessary work and additional headaches during future revisions. Plus, it is so much more elegant!
4.Instances of a Linear Component Pattern Can Now Rotate Along a Pattern Direction
This will be an instant time-saver for many industrial or interior designers. There are just five new elements in the Property Manager of a linear component pattern:
- One checkbox to turn ON or OFF the Rotate Instances functionality
- A field for selecting the rotational reference
- A box for reversing the direction of rotation
- An input field for the angle increment
- A checkbox for aligning instances with the seed (which, if checked, would give the user the choice of placing the reference point in the bounding box center or the component origin)
This is another enhancement that could be considered “small” at the first sight, but seems bigger if you take a look at the difference between the feature tree of a model built the traditional way (using copy with mates) and the one built using the new pattern functionality in Figure 16.
5. Ability to Access the Measure Tool When Other Commands Are Active
This is probably the smallest addition to the User Interface in 2018—a thumbtack—but what a difference it makes in a user’s productivity.
As shown in Figure 17, a user measures the depth of the pocket to calculate the proper offset from the bottom face, without needing to cancel the command in order to access the Measure tool.
The Measure tool received several other enhancements, including:
- Increasing the number of items in the list selections from three to six
- Adding Quick Copy to memory functionality for any numerical measurement
- Adjustable font size
6. Assembly Open Progress Indicator
This “small” enhancement will be welcome by users who work with large assemblies that take longer to load.
Until this year, users were able to provide little or no feedback about what goes on inside SOLIDWORKS during the opening process. Sometimes, a user might even terminate the SOLIDWORKS process, suspecting that the software hanged, when in reality it was still computing, but not communicating with the interface. When users call Tech Support complaining about crashes, a quick check of their application logs would reveal multiple crashes initiated by the user. Productivity is greatly affected; hours could be lost with unnecessary wait and crash cycles.
In SOLIDWORKS 2018, there is a new Assembly Open Progress Indicator, which solves this problem.
The information displayed contains:
- The three major opening phases for the assembly:
- Loading top-level assemblies and reference documents (indicating the name and path of the document that is being processed)
- Updating assembly (computing mates, assembly features, patterns and in-context entities)
- Computing the model tessellation into graphics triangles
- Elapsed time
- The amount of time required to open the assembly, as well as the last time it was opened
For assemblies that take longer than 60 seconds to open, the indicator remains visible after the assembly opens.
7. Ability to Temporarily Hide Faces When Applying Mates
This is such a “small” enhancement that many users would not even notice it. And that is too bad, because their productivity could be enhanced when applying mates to obscured entities.
In essence, the new functionality mimics the Select Other tool, but on steroids. Once the mate command is active, a user could temporarily hide any face the mouse is hovering over by pressing the Alt key.
Every time the Alt key is pressed, another face will be hidden, like peeling layers off an onion. Once the desired entity becomes visible, it could be selected with the mouse to be used in the mate.
Once you practice this technique a few times, the time savings of this enhancement is quite impressive.
8. New Option for the Hole Wizard to Preserve Sizes and Settings When Changing Hole Type
This enhancement addresses a major complaint users had of the Hole Wizard. Imagine you would like to replace a M5 counterbore hole for a hex bolt, with a M5 countersink hole for a flat head screw.
In the past, the Hole Wizard was designed to remember the hole size and settings used the previous time the software was used, for each type of hole. In effect, most of the time, the user would have to redefine the hole size and settings whenever they changed the hole type.
In SOLIDWORKS 2018, there is a new option in the Tools/ Options/ Hole Wizard/ Toolbox that changes this behavior. It attempts to match the size settings of the last hole type used and the size settings available for the new hole type.
The benefits are not limited to the time saved by not having to unnecessary recustomize the hole, but also from eliminating the frustration users experience when their train of thought gets derailed.
9. Ability to Mirror Sketch Entities Using Planes and Planar Faces
How many times have you felt forced to draw a construction line and constrain it to a plane, just because the mirror command would not accept the plane as the symmetry reference?
Good news! The problem has been solved in the 2018 version!
The resulting sketch entities would get symmetric constraints in reference to the plane.
Be aware that currently, there is still an unexpected limitation, where by selecting two entities and a plane, you cannot apply a symmetric constraint.
Overall, this is a great time-saver. My only reserve for this functionality is the introduction of an element external to the sketch in the constraining scheme. A construction line is highly visible and, even if loses its references and dangles, it would still be an easy fix. Missing a plane might take a bit more troubleshooting for an inexperienced user.
10. Smart Dimensions No Longer Automatically Apply to Preselected Entities
Since its introduction in 2016, the fact that a dimension would be automatically applied to preselected entities frustrated many users. This situation was worse for those of us who use the shortcut toolbar (“S”-key) in conjunction to the context toolbars.
Imagine that you just preselected two lines, applied a perpendicular constraint, and then called the Smart Dimension tool to apply a dimension elsewhere. In SOLIDWORKS 2017, the tool would try to apply an angular dimension between the preselected lines. As direct consequence, many users have abused the Escape key in the past two years.
In SOLIDWORKS 2018, the Smart Dimension tool on the context menu no longer supports preselection. If you want to add a dimension to your selection, use the Auto Insert Dimension on the context menu. The Auto Insert Dimension tool automatically inserts the most appropriate dimensions for sketch entities.
The entities supported by the dimensioning tools on the context menu are as follows:
- Line: Linear dimension
- Arc: Radial dimension
- Circle: Diameter dimension
- Two lines at an angle: Angular dimension between entities
- Two parallel lines: Linear dimension between entities
- Arc or circle, and line: Linear dimension between line and center point
- Point and line: Linear dimension between line and point
- Arc or circle, and point: Linear dimension between point and center point
- Arc/Arc or Circle/Circle or a combination thereof: Linear dimension between center points
11. New Ability to Select Over Geometry
As you can see, we continue to list only “small” enhancements. The 11th one solves a major problem that primarily affects users who work with surface modeling, mold design or assembly modeling.
Imagine that a user would need to select only the red reflectors in this assembly shown in Figure 25 directly from the graphic area.
Logically, the user would use the lasso selection. In SOLIDWORKS 2017, the user would be forced to start the lasso from outside the model; otherwise, the first face clicked on would be selected, and the lasso could not start.
In SOLIDWORKS 2018, this behavior can be modified by simply pressing the “T” – key.
What then occurs is shown in Figure 27.
It might not look like a significant time-saver, but such selections are performed tens or hundreds of times every day by some users. Even if a user would save 10 seconds per selection, the time savings could add up quickly, so by the end of the day, a person could have saved minutes or hours.
12. Ability to Import Product Manufacturing Information (PMI) from STEP AP242, CREO and NX
For users who work with customers and vendors using other CAD systems, this new functionality eliminates the need to waste time comparing the model with the 2D drawing. Moreover, it eliminates the danger of the model and drawing being in different revisions.
It also unlocks one more limitation in regard to migrating to a model-based definition (MBD) system.
13. Misaligned Concentric Mates
There is a passionate debate going on in the SOLIDWORKS Forums about this new functionality.
Some users strongly dislike it, believing that it encourages laziness and carelessness when creating and mating accurate models.
In my opinion, the tool would be very useful when working with imported geometry, in which holes could sometimes be less than a micron out of alignment due to import tolerance.
This functionality could also be used as a great troubleshooting tool.
Example: Many users would apply one concentric mate and a parallel mate in order to ensure that no concentric mates would fail. By doing so, they miss out on a critical diagnostic tool: when applying two concentric mates, if you have a misalignment, you want to know if a mate would fail!
The new functionality for misaligned concentric mates solves this problem brilliantly, and it goes even further, considering that users could set the acceptable limits for the misalignment.
For those who do not like this functionality, it can be turned off through System Settings as shown in Figure 29.
So, what goes on when you mate misaligned holes with this new mate? Following are a few things to consider ahead of time:
- Set the maximum deviation and the “default misalignment” behavior in the document properties as shown in Figure 30.
- When applying the mate, I discovered three critical things, which are not intuitive or documented anywhere:
- The mate does not allow for dynamic pivoting of the components inside the misalignment tolerance. That would be nice, but it does not work. If you need to see a part moving to simulate the clearance between a pin and a hole, use a limit distance mate between the two axes.
- Between any two components, you could have only 1 misaligned concentric mate as shown in Figure 31.
- The plane defined by the axes of the first component’s group of 2 holes is coincident with the plane defined by the axes of the second component’s group of 2 holes.
Figure 32. The two concentric mates (1 misaligned) fully define the component in the X-Y direction. A third angle mate would fail, even though it should work physically, given that it is inside the misalignment tolerance.
SOLIDWORKS took great care to ensure that this mate will be as safe as possible. The safeguards are:
- Allowing CAD admins and users to deactivate this functionality (see Figure 29)
- Defining a maximum misalignment deviation (see Figure 30)
- Warning the user that the holes are misaligned before the mate is applied (see Figure 33)
- Identifying a misaligned concentric mate through a specific icon (see Figure 31)
- Validating the design using the new Design Checker rule (see Figure 34)
In conclusion, this could be a great time-saver when working with imported geometry, or when using smart mating schemes for troubleshooting hole misalignments.
14. Full Control for the Tangency Direction of Certain Curved Entities
In the process of conceptual design, before sketches are fully constrained, users experiment with the final shape, size or orientation of sketch components. When doing so, it is possible for the tangencies to flip, as shown in Figure 35.
In the past, users would delete the offending arc and recreate it, which could be costly if other features or mates would had depended on it.
In SOLIDWORKS 2018, the solution is simple and elegant. Just select the arc with the right mouse button and choose Reverse Endpoint Tangency from the menu.
The result is as would be expected (see Figure 37).
15. Show a Document’s Last Open Time in Windows Explorer
This is a great “small” enhancement for all users who are wondering how long it would take to open the file just received from a colleague, customer or vendor. “Do I have time for a coffee? Should I open it overnight instead?”
When you hover over a SOLIDWORKS part, assembly or drawing document in Windows Explorer, a tooltip displays how long it took to open the document the last time it was opened.
Be aware that the data is available only for models that are opened directly from disk and Last Open Time does not update in reference files when they are saved while open in memory, but it does update when the reference files are saved while open in their own window.
A column could also be added in Windows Explorer to see SW Open Time for all files. I recommend using this information in conjunction with the column SW Last saved with.
16. Ability to Insert 3D Views Directly in a Drawing
The 3D Views are the Holy Grail of displaying models in SOLIDWORKS. Unfortunately, they can be created only by users who have access to a seat of SOLIDWORKS MBD. That being said, once3D Views are created, any user can take advantage of them, with or without MBD.
3D Views are so efficient because they act as shortcuts to:
- Display states
- Section views
- Annotations’ visibility
Imagine being able to save all these settings in one place. Until now, they could be used in parts, assemblies, eDrawings and 3D PDFs, but not on SOLIDWORKS Drawings.
Starting with SOLIDWORKS 2018, this limitation has been lifted, opening opportunities for companies using traditional 2D drawings to consider acquiring seats of MBD to take advantage of this great time-saver.
The existing 3D Views from a model are automatically populated in the View Palette, and could be dragged on the sheet, as drawing views. Moreover, any annotations contained in the 3D View could be automatically inserted, if they are orthogonal to the drawing view.
Again, this is a “small” enhancement that could eliminate most of the work needed for detailing in the 2D drawing environment.
17. Smart Explode Lines
The Exploded View functionality was perfected in SOLIDWORKS 2016 and 2017, but exploded lines have not been improved since they were introduced.
I heard many users complaining about the amount of work needed to create and edit exploded lines.
SOLIDWORKS 2018 introduces a revolutionary solution—a completely automated process for the generation of exploded lines.
The workflow is simple and intuitive. Just select an Explode View with the right mouse button, then choose Smart Exploded Lines.
The Property Manager of the Smart Explode Lines tool is also easy to manage as shown in Figure 42.
The user could select all components, or only some of them, and also could select parts or full subassemblies.
The route lines could be automatically drawn between bounding box centers, component origins or user-defined points.
Smart Explode Lines could easily be converted to regular sketch lines in bulk, or one by one.
To convert all lines, right-click on the 3D Sketch of the Explode View and select “Dissolve Smart Explode Lines.”
For one-off conversions, edit the sketch first, then preselect the lines you want dissolved, right-click and choose “Dissolve Entities.”
This “small” enhancement could save hours for a complex assembly, and even more time for revisions.
18. Ability to Mirror Entities in a 3D Sketch
The two sketching environments, 2D and 3D, have had differences in functionality for a long time. That might be explained by the different “engines” used by each of them, the D-Cubed 2D DCM and D-Cubed 3D DCM (find this information in the HELP/About menu).
One of the major limitations for 3D sketches was the inability to mirror entities. Logically, a 2D line could not be used as a reference for 3D mirroring, which need a plane or planar face instead.
As you know, after reading enhancement number 9 on this list, planes and planar faces can now be used in the mirroring operation for 2D sketches.
The good news is that this functionality extends to 3D sketches.
The major beneficiaries of this new functionality are the users who work with the weldments and/or routing environments.
19. Online Licensing
Until this year, companies had two choices for managing their licenses. They could either install stand-alone licenses, where the activations are tied to machines, or network licenses, where the activations are managed at the internal server level.
What happens when a user visits a customer, but his or her machine is not located onsite?
Starting this year, there is a third option for accessing your SOLIDWORKS seat, called Online Licensing. Online Licensing will allow a license to “follow the user” instead of staying on an activated machine. Anybody using SOLIDWORKS 2018 with a Standalone license will be able to use Online Licensing.
To turn Online Licensing on, a user needs to access the new SOLIDWORKS Admin Portal, select a product, and switch the activation type from “Machine Activation” to “Online Licensing” (see Figure 46).
The product will need to be deactivated first if it has been installed and activated previously.
Products can then be assigned to individual users (see Figure 47).
After installing SOLIDWORKS, the next time the user launches the program, they will just need to log in using their SOLIDWORKS ID.
The good news is that a user does not have to log in every time they use SOLIDWORKS. Moreover, when accessing the software on a different machine, they could easily disconnect the first session (without losing their work).
Who this new licensing model is best for:
- Users who want to move freely between all their devices
- CAD admins who want to easily add/remove products to their users
Who this new licensing is not best for:
- Users with bad Internet connections (not related to the bandwidth, but to interruptions)
- If there is an Internet connection at startup, but it gets lost in the middle of the session, a warning will pop up telling the user to fix the connection before an eventual shutdown occurs. The warnings would start to appear around 10 minutes after a connection is lost.
- The user must be online in order to use the license offline. A user will still need to remember to be online that before they leave the connected world.
20. Extracting Geometry from a Corrupted Solid Body
File corruption primarily affects users who work directly over the network. If there is a network hiccup during a file-saving operation, files could be corrupted.
In the past, a corrupted file would have been unusable. Sometimes, a value-added reseller (VAR) could attempt to recover some information, but that is a time-consuming process.
Starting with SOLIDWORKS 2018, when the software attempts to repair a corrupt file and cannot resolve the problem, the user would be given the option to extract geometry (if the body data of the file is still intact). If the option is accepted, the software imports the geometry from the corrupted file into a new file.
In effect, the user would get a similar model as the one generated by importing geometry from a neutral file.
The file could be mated, material and properties could be assigned, and the file could be also further edited using standard SOLIDWORKS features.
When you attend a launch event delivered by your VAR, or just read the What’s New Document, do not ignore the “small enhancements” in SOLIDWORKS 2018. As you read in this article, this year, small changes can add up to big productivity!
About the Author
As an Elite AE working for Javelin Technologies, Alin Vargatu is a Problem Hunter and Solver, and an avid contributor to the SOLIDWORKS Community. He has presented 19 times at SOLIDWORKS World and tens of times at SWUG meetings organized by four different user groups in Canada and one in the United States. Vargatuis also very active on SOLIDWORKS forums, especially on the Surfacing, Mold Design, Sheet Metal, Assembly Modeling and Weldments sub-fora. His blog and YouTube channel are well known in the SOLIDWORKS Community.