Don’t Close Yourself Off: Close Sketch to Model in SOLIDWORKS

SOLIDWORKS users, after enough time learning the program, tend to get into habits. They use generally the same commands from one day to the next, browsing through the same toolbars and tabs or creating shortcuts to locate what they need. Aside from occasionally having to find an atypical command for a one-off kind of feature, our emphasis on efficiency and productivity makes it so that most users don’t spend much time exploring the program’s menus. As a result, there are some tools in SOLIDWORKS that simply do not get used very often.

I was recently teaching a user looking to get refamiliarized with SOLIDWORKS after working with a different CAD packages for the past several years, and at one point they asked if SOLIDWORKS has a tool or a hot key of some sort that could automatically close open sketch profiles. Other programs seem to have this functionality or something similar, but my initial instinct was, no, SOLIDWORKS does not have such a feature. However, in the process of searching for a comparable command, I found an interesting tool that I had honestly never seen before: Close Sketch to Model.

Close Sketch to Model will take an open profile whose endpoints are coincident to edges of a face and convert portions of that face into the sketch to produce a closed profile. Like many underutilized SOLIDWORKS commands, it can be found in the extensive Tools > Sketch Tools menu.

Launching the command presents a simple popup dialog, allowing you to specify which of the two possible directions you want the closure to follow, indicated by arrows attached to an endpoint of the sketch.

Once you hit “Yes” to end the command, the necessary edges will be converted into sketch geometry and secured in place through an On Edge relation. (The relations appear graphically as Offset Entities relations until you exit the sketch, but looking at them through the Display/Delete Relations viewer will show that they are On Edge.)

It is worth recognizing what SOLIDWORKS does in the background here. To create the sketch shown above, Close Sketch to Model is essentially converting all four edges of the model into the sketch and trimming them where needed to produce the closed contour. In other words, a procedure that would normally require a Convert Entities followed by a Trim Entities can be reduced to one automated step. This can be a major time-saver, especially when you consider how tedious the process of manually selecting edges to convert can be.

Additionally, the geometry you are trying to close to does not need to be on the sketch plane. Just like Convert Entities can be used to pull geometry that is in front of or behind the plane into your sketch, Close Sketch to Model can project entities onto the sketch plane. The critical step here is that you have added Coincident relations between the sketch endpoints and the relevant edges. These relations help SOLIDWORKS identify which edge loop you are looking to reference with the command.

Close Sketch to Model is not a new function or anything; I could find entries in the Help documentation for it going back to SOLIDWORKS 2010 (as far back as these files go). Still, there is next to no information for it online. This is largely due to the command’s obscurity in the menu structure, I suspect. (It should be noted that you could program a keyboard shortcut through the Customize dialog if you want easier access to this tool in the future!) Were it not for the student in my class who asked me about it, I would likely never have noticed. Even as someone whose job is to constantly learn about SOLIDWORKS, there are some things inside the program that surprise me.

I hope this encourages you to try digging through the menus sometime. Obviously you have work that needs to be done, but there is a possibility that you will uncover something that ends up saving you time and effort in the future. So, maybe during a lull when things aren’t too busy, take a few minutes to explore. If you browse with an open mind, you might even come out of it with a closed sketch.

Anthony Sandri
Application Engineer
Computer Aided Technology, Inc.