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The house I grew up in was a Mexican colonial style, with beautiful wrought iron fences and gates surrounding the yards. There were also wrought iron details on stairs, windows and doors.  Here in my neighborhood I’ve found only houses with backyard fences made out of wood, and no fence in the front yard. They look nice, but at times I kind of miss the elegance of the wrought iron fences of my childhood. Maybe that’s why I decided to make this for my very first experiment with SolidWorks weldments.

As I found out, most of the time, when working with weldments, you will need to create a sketch that will work as a layout or skeleton of your design.  You also need a second sketch, known as a weldment profile, and that is actually a Library Feature kind of file (.sldlfp). Think about a sweep feature for a moment; the weldment profile will be swept along the path you specify with your layout or skeleton sketch. In the following image, for instance, the line in blue corresponds to Sketch 1, the layout sketch, and the sketch in pink is the weldment profile that is being swept along Sketch 1.

Layout sketches can be 2D or 3D sketches, but they must contain only lines and arcs, no splines.  As for the weldment profiles, SolidWorks provides a few, and others can be downloaded from the internet (subscription service members only), by clicking on the Design Library tab on the task pane and then on SolidWorks Content, and opening the Weldments folder. Once there, ctrl + click on the zip file of weldment profiles you wish to download, unzip the files, and make sure to add the path to their location on Tools, Options, System Options, File Locations, Weldment Profiles, so you can access the weldment profiles in SolidWorks. 

You can also create your own weldment profiles, and that’s what I ended up doing, since I couldn’t find one suitable for what I had in mind. Creating a weldment profile isn’t hard, but there are a couple of things you need to keep in mind.  The first thing to consider is that the origin of your sketch will automatically become the default piercing point of the profile, so you better take advantage of any symmetry your profile may have. The second thing to consider is that later on, while using the profile to create structural members, it will be possible to select any vertex or sketch point as an alternate piercing point, so make sure to plan for it.

So, with this in mind, the procedure for creating a weldment profile is quite simple. Open a new part, create your sketch, and then save it as a Library Feature Part (.sldlfp) in a location where SolidWorks will be able to access it later. This is one of my custom weldment profiles. As you can see, it’s a very simple shape of the cross-section of a rectangular rod.

Once I had my custom profiles ready, I made my first sketch on the Front plane. The circle you see there isn’t actually a closed entity; I used Split Entity on it, or else it wouldn’t work out as a path to create a structural member.

On the weldments toolbar, click on the Structural Member icon and this will open a property manager that allows you to select the weldment profile you wish to use, the path, and even the orientation of the profile, by rotating the sketch or changing the piercing point. In my case, I’m choosing one of my custom made profiles, Sq. 0.5.sldlfp that I saved in a folder called Created Rods. As path segments, I chose the two vertical lines in the sketch.  Notice that the same sketch can be used to create different structural members.

I can now use the rest of the sketch to create other structural members in a similar fashion. I start by choosing one of the arcs in the design in the middle. I want it to be one structural member, rather than three smaller ones, so after I select all three arcs, I make sure I mark the option Merge Arc Segment Bodies in the property manager.

Notice in the image that I need to reorient this particular profile.  I begin by rotating it 90°.

This works better, but I have interference with the other structural members. I can solve this by clicking on Locate Profile in the property manager and selecting a different pierce point in the sketch, one on the edge of the profile, instead of the origin. In the image, the point in pink is the current pierce point, the point in orange indicates that the point can be chosen as the new pierce point.

Here is the result of this last operation, plus doing exactly the same for the circular sketch in the middle.

Notice how each time a new structural member is created it’s also added as a new body, and listed under Cut List. This is, in fact, a multibody part with four different bodies, so far.

The rest of the structural members in the fence are created in a very similar fashion, using a couple of other custom profiles of mine, the four sketches shown in different colors in the following image, and the Linear Pattern feature (keep in mind that we are patterning bodies here). Notice in that same image that there’s now twenty five bodies listed under Cut List.

This post is way too long already, but in a future one I’ll show you what to do with that Cut List and how to use it in a drawing document.

So, what do you think? Is that a nice fence or what?

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