‘Impossible’ Modeling Challenges Solved by CAD Power Users

The Backstory

If you were to ask what the most important quality of SOLIDWORKS is and expect me to rave about the exceptional ease of use, intuitive interface, rich ecosystem or speed to which I can model most everything with it, my answer could surprise you. Yes, I acknowledge all the above. For me, the biggest advantage, as a SOLIDWORKS user, is being a member of a huge and passionate community of users.

My job title is process improvement consultant for Javelin Technologies in Canada. When I am asked what my job entails, I reply that I am a problem hunter—solutions architect. When a company defines goals for its engineering team like doubling productivity, eliminating errors or reducing repetitive tasks, my role is to hunt for any problem that could prevent them for reaching the goal and then design a custom solution for solving it.

It is true that many problems are similar for most engineering teams, regardless of the type of product they design or industry they serve. For example, large numbers of engineering managers would mention large assembly slowdowns affecting their team. While the symptoms are the same, the causes are, most of the times, unique for each team. Finding these specific causes and tailoring solutions for each customer is art as much as science.

Throughout my years as a hunter, I had the opportunity to add exotic trophies to my collection of challenges experienced by end-users. I found the most interesting ones when the existing SOLIDWORKS functionality could not provide a direct answer to the problem. A new method, technique or workaround had to be designed.

After finding a solution to each problem, I could not refrain from wondering whether an even better solution existed. And, where else could one find brain power capable to solve such challenges other than the place where the best SOLIDWORKS power users are known to congregate? Of course, I am referring to the SOLIDWORKS Forum.

What Are SOLIDWORKS Power-User Challenges (SWPUC)?

… and this is how the idea for SWPUC was born.

Other than having fun solving riddles, the declared goal of SWPUCs has always been to facilitate—through brainstorming—the finding of new techniques and methods for the benefit of the SOLIDWORKS community.

The participants strive to:

  • Identify areas where SOLIDWORKS’ functionality needs enhancements.
  • Design workarounds to overcome the current lack of functionality.
  • Submit new enhancement requests (ERs) or promote existing ERs, relevant to each challenge’s topic

Since May 17. 2017, modeling challenges have been posted on the forum. Each of them received multiple solutions. At the end of each challenge, the users who submitted the best solutions received the title of SOLIDWORKS PowerUser, along with a certificate signed by three peers.

As a side note, the artwork decorating the border of the Power User certificate has a unique story worth its own article. It has been created by one of the top forum contributors, John Stoltzfus, using SOLIDWORKS as the medium.

Sample of a SWPUC certificate.

What Is a SOLIDWORKS Power User?

We asked the winners of the SWPUCs to come up with a definition for a Power User. This is what some of them wrote:

Who Cares about the SWPUCs?

My first answer, somewhat selfishly, would be “my customers.”I actively share any new solution resulted from crowdsourcing on the forum with customers who would benefit from it.

When this question was directed to the forum users, it became clear that the benefits extended to the user community and SOLIDWORKS as a company. Everyone benefits:

  • Power Users who participated in the challenges.
  • SOLIDWORKS forum participants who find answers to old questions. Most of the problems are relevant to specific groups of users.
  • SOLIDWORKS as a company benefits from the limitations identified in the challenges and enhancement requests that are created at the same time.
  • The whole SOLIDWORKS community, once SOLIDWORKS implements solutions as per point 4.

This is sample of what users wrote:

The first article in the SWPUC series describes the first challenge and its winning solution.

Challenge 1 – Simulate a “Point Captive on a Face” Mate

A common mating problem in SOLIDWORKS is attempting to limit the movement of a pin in a groove by the physical interactions between the two components.

The blue pin should be allowed to move anywhere in the white space of the groove.

Currently, SOLIDWORKS functionality allows it to simulate the movement of the pin without using a mate. The Physical Dynamics mode in the Move Component command could be use for that.

Physical Dynamics.

The pin should be free inside the groove.

The problem with Physical Dynamics is that it is active only as long the Property Manager for the Move Component command is on. That is not enough for most users’ applications. They want to be able to simulate the movement all the time using mates.

Since there is no volume mate in SOLIDWORKS, the first thing users attempted to do was build a construction face in the yellow part, representing the space where a point on the axis of the blue cylinder could be restrained on. The simplest way to achieve that is by creating a planar surface from an offset contour, with the offset equal to the pin’s radius.

Attempt 1 – Building the “trap.”

Back to the assembly, it seems intuitive to believe that applying a coincident mate between a point on the axis of the pin and construction face would solve the problem.

Mate the point on a planar face.

Unfortunately, for algebraic faces, the boundary considered by a Coincident Mate is the full untrimmed surface. For a planar face, that is the whole infinite plane.

The planar limit is infinite in this case.

The good news is that this problem could be easily diagnosticated using the Untrim Surface command.

A simple test: run the Untrim Tool.

The next workaround users tried was deforming the construction face using the Dome, when the face belongs to a solid body, or Freeform feature.

Using Freeform to deform the planar surface.

Unfortunately, the resulting surface is still untrimmable, which would make the point free to move anywhere on the untrimmed surface.

Deforming a planar face would deform its original fabric, without limiting the boundaries to its edges.

If only the deformation would go in one direction only, either above or below the original plane. In that case, we could apply a Limit Mate that would constrain the point on one side of the zero value.

So, what is the solution that works?

It starts with building an untrimmable face. Such a face could be created by using one of the algorithmic type of surfaces which could be produced with tools like Loft or Boundary Surface.

In this example, a plane was created for the purpose of adding a curve to define the new surface.

First step in preparing a non-planar, untrimmable surface.

A simple arc is added, with Pierce relations to the lines of the groove.

The mating face was defined as a boundary surface.

Notice the use of the Selection Manager for defining groups of curves.

Let’s put the new surface to the test using the Untrim feature. This way, it is easy to demonstrate that SOLIDWORS cannot extrapolate the surface any further.

The new surface is not trimmed from a larger fabric.

Returning to the assembly, if we want to ensure the pin does not move up and down on the new construction face, it is worth adding a new construction component.

The origin of the new Link component is mated coincident to the construction surface.

Now, let’s add a second coincident mate to the Link’s origin. This time, we will mate it to the axis of the cylinder.

The final goal has been achieved, A point on the cylinder axis is captive on a surface with edges that are a cylinder radius away from the groove’s faces.

The last step is hiding the construction surface. Once that is done, the cylinder can be dragged anywhere inside the groove. It will never interfere with the yellow plate.

The Pin-in-the-Groove mate has been applied.

Conclusions and Deliverables after the First SWPUC

    • Limitations identified in the current SOLIDWORKS functionality
      • The edges of a face do not represent limits for a Coincident Mate.
      • The underlining (untrimmed) surface is used for defining a Coincident Mate.
      • The underlining surfaces for some algebraic faces do not have limits (planar, cylindrical, conical).
    • SPR Recorded by SOLIDWORKS as a Direct Result of the First SWPUC

SPR 1051495: Add the functionality for Lines and circles to terminate movement of objects mated to them with a coincident mate like the splines

    • The 10thIdea Voted in the Top Ten at SOLIDWORKS World 2018

Add option to limit Coincident mate to area of face selected for all types of face.


    • Video Demonstration

You can use this link to watch SOLIDWORKS Tutorial: Mating a Free Pin in a Pocket, Real Life Conditions, a video demonstration of this technique.

The Winner of the First SWPUC

John Stoltzfus

Product Development Specialist

Keystone Collections

John Stotzfus has been using SOLIDWORKS since 1997, primarily for Custom Dry Bulk Material Handling Equipment Industry and Custom Fabrication, using Sheet Metal with Assemblies of over 4,000 components.

Since 2014, Stotzfus has used SOLIDWORKS to design custom furniture. For that, he developed an efficient Skeleton Sketch Top Down design approach, which enables changes to be made simply and easily.

Stotzfus is also an accomplished artist who uses SOLIDWORKS to create abstract art.




Stay tuned for the next articles in the SWPUC series, demonstrating more original solutions to “impossible” modeling challenges in SOLIDWORKS.


About the Author

As an Elite AE and Process Improvement Consultant, working for Javelin Technologies, Alin Vargatu is a Problem Hunter and Solver, and an avid contributor to the SOLIDWORKS Community. He has presented 22 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. Alin is 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.

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