When Boundary was first released, it looked like a mostly redundant Loft feature. However, as the details of the new feature slowly came into focus through a lot of trial and error, comparison and research, Boundary quickly gained traction—and eventually won out over the Loft feature among those who work with surfaces daily.

Boundary has several advantages and differences when compared to the other interpolating features Loft, Sweep and Fill. Spoiler alert: Boundary is the first feature that many—maybe even most—SOLIDWORKS surface modelers use when called on to make a complex shape.

Accuracy

One of the advantages of the Boundary feature that the developers explained during the initial release was that the accuracy of the Boundary surface compared to the sketched curves is better for Boundary than for other features (except Fill). Before Boundary, many surfacers would complain that sometimes a surface resulting from multiple profiles didn’t actually touch the initial profiles. These profiles could be sketches, edges or curve features.

Loft and Sweep approximate profiles, especially non-spline shapes, which get converted to splines. Boundary may still do this, but it does a better job and approximates closer to the input geometry. This was a big deal, and helped propel Boundary over Loft.

Equality Between Direction 1 and Direction 2

Another factor that distinguishes the Boundary feature is that it treats Direction 1 the same as Direction 2. We all know that most surfaces in CAD are based on NURBS, and NURBS depends on a 2-directional U-V mesh of.

On a Sweep, one direction is called the path and the other direction is called the profile. On a Loft, one direction is called the profile and the other is called the guide curve. But in the Boundary surface, you just have Direction 1 and Direction 2, and they both have exactly the same controls. The Loft surface only allows you to apply Curvature Continuity (C2) to the beginning and the end of the loft, not to the sides.

The importance of the equality of the directions is shown in this example. We have the following shape with a hole in it that needs to be completed (without using the Delete Hole or Fill features). Let’s use Loft, and then Boundary.

Figure 1: Original Surface.

Figure 2: Loft patch, not as nice as the Boundary patch.

From these images, you can see from the smoother zebra stripe display that the Boundary surface patch (on the top) is able to get good results with Curvature to Face in both directions. Loft can only manage to use Tangency in both directions, and the zebra stripe display is not very good. Even though Curvature is available in the Profile constraints, Loft cannot make it happen when guide curves are also selected, and tangency is the only option available for the guide curve constraints.

A sample file for this is available in SOLIDWORKS 2020 format at this link.

Arrangements of Curves

The Boundary surface allows a bigger range of arrangements of curves compared to the Loft. Loft requires at least two profiles, but it can work with or without guide curves. Boundary requires at least two curves, and doesn’t care about which directions or combinations. It can use one Direction 1 and one Direction 2, or two Direction 1, or two Direction 2.

Loft also ends the surface at the profiles, and it won’t give you any extra surface if your guide curve extends past the profile. So, the curves might look like the lines in the letter T, L or E, but you could use an arrangement of curves that looks like an X or #.

For example, using the mesh of intersecting 3D splines shown below, with the purple being guide curves (Direction 2), and the blue being profiles (Direction 1), the resulting Boundary surface uses the complete length of curves in both directions, while Loft only uses the entire profile, but not the guide curve.

Figure 3: Original mesh of curves.

Figure 4: Loft doesn't make use of entire length of guide curves.

Figure 5: Boundary makes use of entire length of all curves unless the Trim By Direction options are used.

Also notice the difference in the callout flags; Boundary allows you to use them to set tangency conditions, while Loft does not.

Boundary also has the often-overlooked option called Trim By Direction. So, you could have a ‘#’ arrangement, and then trim it back so that it only gives the center square as a result, or it might also give an ‘H’ type result. Trim By Direction can be useful, especially when you are using existing edges as profiles. You can download this mesh example from this link.

Figure 6: Trim By Direction allows you to decide how much of which curves to use.

Connectors

Boundary also allows you to use Connectors in both directions, whereas Loft only allows this in one direction. Connectors are like ad hoc guide curves, and they are the reason why you don’t hear the old lie about how “your loft profiles need to all have the same number of segments” anymore. Connectors are very powerful. Sometimes they can be the difference between a Boundary working and not working, and sometimes they can allow you to change the flow of a feature subtly, to make it really the right shape.

In the image below, the connectors are the purple dots that connect between the purple curves. In this case, the connectors help keeping the U-V sections lined up as the surface transitions around the bend. The alternative to using connectors is drawing a lot of profile curves. The connectors can be edited on the fly while the Boundary command is active.

Figure 7: Connectors help you control the flow of surfaces.

Internal Profiles

It is common to control the tangency of the first and last profiles on a loft or boundary. Sometimes you need to control the tangency direction of an internal profile. So, maybe the second of three profiles needs you to control the direction. Usually, you would do this with Direction 2 curves, but it never hurts to have more control. Try to place internal profiles to match the flow of the feature as best you can, but there are times where you need a little extra help.

Special Functionality

Degenerate Surfaces / Loft To Point

Degenerate surfaces are surfaces where all of the lines in one direction, U or V, come together in a single point—like at the North Pole on the globe. This is a situation you find in CAD models from time to time, but sometimes it causes problems. It can cause problems with offsets, shells, fillets and other types of features.

Both Loft and Boundary enable you to create this type of geometry, where the profile on one end is just a point. The typical example of this is a surfboard. When shelling out a model like this causes a problem, the typical solution is to cut off the degenerate end, and replace it with a Fill surface, which will be the topic of a future article. You can download this sample file at this link.

Figure 8: Degenerate features can be useful, but can also cause issues with other downstream features such as shell, offset and fillet. Boundary and Loft can both create features that terminate in a tangency to a point.

Drag Sketch

Drag Sketch is an option that is only available when all of the curves in the active Boundary (or Loft) feature have been created in a single sketch. This is usually 2D or 3D splines in a 3D sketch. It lets you dynamically drag sketch points as the surface updates. The option is found in the PropertyManager. This is very helpful for visualization while creating or editing surfaces. Download this sample file at this link.

Tangency Weighting / Apply To All

Tangency weighting allows you to control the strength or stiffness of tangency end conditions. It works similar to the tangency arrows at the ends of splines. The image shown below only uses two profiles, but the tangency weighting arrows are controlling the shape of the feature.

Figure 9: Tangency weighting can help you control the shape of a feature without adding curves.

Figure 10: The weighting strength directions can interact and give interesting shapes.

The Apply To All option is on by default. This means that any tangency weighting you apply to a curve applies to all nodes of that curve. If that option is turned off, then you can change the weighting for each individual node of a curve, as shown below. The nodes at the close end of the curves are set to heavy weighting, while nodes at the far end are set to weak weighting. This allows you a lot of control in certain situations where you might need extra flexibility without adding additional curves to your feature. Download this sample part at this link.

Curves Influence

The Curves Influence options depend on the type of profiles you have. If you have profiles with sharp corners, or multiple segments, it can give you options that other profiles don’t allow (such as a single smooth spline).

The options are:

• Global
• To Next Curve
• To Next Sharp
• To Next Edge
• Linear

These options mean that the curves in the given direction will affect the overall shape of the feature “globally” or “to the next curve” and so on. If you have a profile such as a rectangle with sharp corners, then the curves will only influence the shape up to the next sharp corner of the curve in the other direction.

Not all of the options apply to every situation. The solutions depend on how many curves are selected in each direction, and if your curves have multiple segments, non-tangent segments or other factors. In most cases, there are only a couple of solutions for all of the options. You might find it best to just cycle through the options and see which one is best.

Disadvantages

It’s not all peaches and cream, however. There are several functions that you can’t get with the Boundary that you can get with Loft.

• Centerline Loft (works like multi-section sweep).
• Closed Loop (you can make a closed loop with Boundary, but you have to use one of the curve directions to create an actual closed loop curve).
• Add Loft Section.
• Separated tangency/directional controls.
• Micro Tolerance .

Summary

The Boundary surface feature in SOLIDWORKS can be as simple or as complex as you want to make it. It is the basic surface type that most users go to when they need to make a complex shape. There are many options you can use like the Drag Sketch to make this feature easier to edit in real time. Many more examples can be found on the author’s subscription site, SOLIDWORKS Surfacing Episodes.

To learn more about SOLIDWORKS, check out the whitepaper Developing Better Products in the Cloud.

After spending years designing with SOLIDWORKS, going to user group meetings and attending the annual SOLIDWORKS World Conference, I have picked up quite a few of these. The funny part is I started to assume that if I knew about a certain technique, then everyone knew about it…right?

As I gave a presentation at a user group meeting or helped a colleague with an issue, it was common for me to hear, “Wait a minute. Back up. What did you do there?” Could it be possible that not everyone knew about all of these little timesavers that I always took for granted? I decided to start compiling a list of my favorite tips and tricks after finding out that some of my favorite power users on the SOLIDWORKS forums didn’t know about several of them.

When it was decided that I would be the presenter for the second annual SOLIDWORKS Largest User Group Meeting Ever (SLUGME), I knew I had the makings of the perfect presentation. One day while jotting down notes for my presentation, I was listening to some tunes, and the presentation found a name – All the Small Things. This is how I often describe the timesaving benefits of shortcuts. “How did you get that done so fast?” “Easy, it was ‘All the Small Things’!”If you are not familiar with SLUGME, it was a crazy idea I had a few years ago to have user groups from all over the globe “connect” to view a single presentation at the same time.

I modeled this presentation around the Jeopardy! game show. Each category had a specific theme. This allowed me to cover a lot of ground and share many great tricks within SOLIDWORKS. My time limit was going to be a little less than an hour, which meant that I would need to move fast to get through all of the categories and topics.

My intent for the presentation was to spend most of the time working in SOLIDWORKS. The individual topics were starting points for small demonstrations. This allowed me to share multiple tips and tricks for each topic. For example, one topic was the “S” key shortcut—this displays a pop-up toolbar, but it also activates the command search. These are two tips from a single topic, but when I did the presentation, I added almost a dozen tips related to the topic. There is not enough room in this article to list every single tip or trick, so I am only listing the categories and highlighting a few of the topics for one of the categories.

Below is a brief description of what was shown for my All the Small Things presentation:

	This category contained several of my favorite keyboard shortcuts.
	This category covered tools for working with tubing.
	This category showed great shortcuts for creating Weldments.
	The random tips and tricks category had a little bit of everything.
	Custom Properties is one of the most powerful tools within SOLIDWORKS. It is also one of my favorite timesavers, so these are some of my best tricks.
	Modeling and filling a bath tub using a number of different tips and tricks. This was a really fun category, so I will go into a little more depth with the topics.
	A few of the multitude of shortcuts, tips and tricks from this topic included: Use the slot tool to sketch the outside shape of the tub. Hold the shift key while selecting the outside of the slot for overall size dimension. When creating the Extrude, use a combination of Offset Sketch, Up to Surface and Draft to keep the tub within the size boundary. The fillet on the bottom of the tub can be made with very little mouse movement. Left-click on the side, use Select Other from the pop-up menu to select the bottom face, select the fillet tool from the pop-up menu, key in a value and select OK. After a quick Shell, the tub is complete.
	Quickly calculate the amount of liquid it will take to fill the tub with a couple tools. Hold Control and drag top plane up to create a new plane representing the water level. Use the Intersect tool to create a new body to represent the volume of water. Uncheck “Merge Bodies” in the Intersect Property Manager to keep all three bodies. In Settings -> Document Properties -> Units -> Custom you can change the units for Volume to US Gallons. Select Mass Properties, and then select the solid body that represents the water to get the volume.
	Now that we know how many gallons of water the tub can hold, we can easily determine the fill level. Right click on Sensors in the Feature Manager tree and select Add Sensor. Select Volume and the solid body representing the water. I set an alert to notify me when the volume was less than a specific value. This way, I can drag the plane up and down until I reach the volume required.
	For this example, I opened a bartender’s drink jigger that I designed using some of the previously mentioned techniques. I calculated several different 1-ounce solids, used the Combine tool to bring them together and used Combine again to subtract them from a solid bar of aluminum.
	This was a really fun way to wrap up my presentation. I showed how to create an animation with the Motion Manager to show the draining of the bath tub. This was a small assembly— the tub, water and a rubber duck just for fun. The water was created by modeling a solid block, using Cut with Surface in conjunction with the inside surface of the tub. The water was mated in the assembly to only allow movement in the Y direction. Open the Motion Manager, drag the time bar to about 5 seconds, drag the water to the bottom of the tub and Calculate the Motion Study. When you play the animation, the water “drains.”

If interested, you can view the entire presentation here or here. I also created a booklet that contains everything from the presentation. More information about the presentation can be found on the SOLIDWORKS forums.

About the Author

Todd Blacksher is the President of the SOLIDWORKS User Group of Nebraska (SwugOne), and is the SOLIDWORKS User Group Network Representative for the Southern US. Todd was named the DriveWorks User Group Leader of the Year in 2016. At SOLIDWORKS World in 2018 Todd was presented the SOLIDWORKS User Group Leader of the Year and the Michelle Pillars Community Award. Since earning his CSWP in 2005, Todd has collected another dozen certifications, the most recent one being his CSWE in 2015. Todd worked for a SOLIDWORKS reseller for a number of years before returning to industry, and resuming his role as President of SwugOne. Jumping on a bicycle and pedaling around as often as possible is a priority for Todd.

What does it take to be a top CAD modeler? How can you rise to the peak of your design game and earn the recognition of your peers? We asked Tom Smith, winner of SOLIDWORKS World 2018’s Model Mania competition, how he found his way to the top.

Meet Tom Smith

Tom Smith coming up the SOLIDWORKS World 2018 stage stairs. (Image courtesy of SOLIDWORKS).

Smith graduated from Stevens Institute of Technology in 1997 as a mechanical engineer. However, it wasn’t until he landed his first job that he began using 3D CAD—specifically, SOLIDWORKS.

“My first job getting out in 1997 was with a very small company,” he said. “There was one guy drawing things by hand and another guy popping it in AutoCAD. I brought in the SOLIDWORKS demo that you could get at the time. You could use it for 30 days. I tried it out, and I’ve stuck with it since then.”

Since he hadn’t learned CAD modeling as an engineering student, Smith learned SOLIDWORKS the old-fashioned way: trial and error. Practice, he explained, was easy to come by.

“When you design things today, usually you go to a website and download the models,” he said.“That wasn’t around back then, so we had to draw everything. Every time you got new bearings, new gear boxes, you got out the calipers and drew everything, and it had to be right. Everyday was modeling things over and over again. You start to get good at it.”

Model Mania

The part that contestants were required to model for Model Mania 2018. (Image courtesy of SOLIDWORKS).

All that practice paid off for Smith. Not only has it served him in his professional career, but it’s won him perhaps the most important prize of all: bragging rights. He has placed in SOLIDWORKS World’s Model Mania competition not once, not twice, but three times, two of those times as the first-place winner.

A tradition of every SOLIDWORKS World since 2000, Model Mania is a competition in which entrants are given a 2D drawing of a part and must model it as quickly and accurately as possible. Competitors are then presented a revision to that part and must make the necessary changes. Winners are chosen based on the accuracy and timeliness of their models. For a convention full of CAD modelers, it’s a fun and popular way to show off their SOLIDWORKS skills.

At the suggestion of a colleague, Smith entered his first Model Mania in 2013. To his surprise, he took second place. The next year, he tried again and one-upped himself, winning first place in the competition.After a three-year dry spell (his own words), Smith reclaimed his crown at SOLIDWORKS World 2018, once again taking first place.

“Model Mania is like real life—you design something, and your boss tells you to change it,” he said. “I’ve been dealing with that for 20 years, so I kind of know what to expect.”

For all you would-be Model Maniacs, Smith was kind enough to pass on some of the CAD wisdom he’s gleaned over the years:

“Don’t leave things under defined. Use major planes, major geometry to stick to. Don’t try to reference sub-features, like fillets. Don’t reference things that will easily fall apart. That’s probably the best trick. If you reference things that aren't going away, like planes and origins, you’re good. If you build to strong reference geometry, your changes will be a lot easier. Another good tip: don’t do everything in one sketch. Split it up. Do fillets afterwards. Keep it simple.

“When you do the contest, they give you two minutes to plan. Take that time to look over the model, build it in your head first and go through the process of what the software’s going to do when you start modeling things so you’re not surprised by anything. Then you start the clock and hack away at it, and just do the best you can really.”

If you’re struggling, it’s good to remember that even the pros have their lapses. He readily admits that when Model Mania host Mark Schneider was going through his solution, Smith noticed a missed opportunity.

“When Mark Schneider was doing the walk-through, he went though the step of doing a shell command,” he said. “And that would’ve saved me like another three minutes, if I’d remembered to do the shell command.”

Mark Schneider’s walk-through of Model Mania 2018. (Video courtesy of SOLIDWORKS).

Thinking Like A SOLIDWORKS Expert

Smith is both a Certified SOLIDWORKS Pro (CSWP) and Certified SOLIDWORKS Expert (CSWE), the highest level of SOLIDWORKS certification currently possible. There are whispers that a new level (SOLIDWORKS Wizard?) might be added, and if so, he will be first in line to take the test.

While he has moved on from being a design engineer—Smith currently runs the SOLIDWORKS PDM system at Victaulic, a provider of mechanical pipe joining solutions—he’s still the go-to guy in the office for SOLIDWORKS advice.

“The designers here give me a call and ask me to help them out if they get stuck on a sheet metal piece or some other wacky model. So, you know, I’m not totally out of it. I’ll sit down with them for an hour and show them how to do things,” he said, jokingly adding, “but it’s nice not to have project managers chasing me.”

Smith spends his spare time modeling and 3D printing his own personal projects, most of them for his hobby of drone racing. An engineer through and through, he still gets his fill of the most important part of any CAD modeler’s education: practice.

“In your downtime, pick something up off your desk, get your calipers and draw it up,” he suggested.