Creating Custom Weldments
Written by: Jared Spaniol, Application Engineer, CSWE
SOLIDWORKS comes with many features and files loaded “out of the box”. This is a great starting point for users, but many times users require more custom sizes to continue with their designs. In the case of the Weldments tool, this can done relatively easily by utilizing pre-existing sizes or creating your own custom sketches if something less common is needed.
First, let’s start with a few basic things to know. The default directory for the Weldment profiles that are included when you install SOLIDWORKS is located here: install_dir:\Program Files\SOLIDWORKS Corp\SOLIDWORKS\lang\english\weldment profiles.
Within that folder you’ll see two folders, ANSI Inch and ISO, that contain a few stock Weldment sizes such as angle iron, c-channel, pipe, rectangular tube, etc. SOLIDWORKS includes a few common sizes for each type of shape, but if you do a lot of designs with Weldments, these will be limited especially if you use any custom shapes or sizes.
When you save a file as a Weldment profile it is saved as a Library Feature Part with the file extension SLDFLP. This is simply done by selecting “Lib Feat Part (.sldflp)” from the drop down of file types (Figure 1). The same is true when you open an existing Weldment profile; you’ll open that SLDFLP file in SOLIDWORKS if you need to edit it.
One thing to note when creating custom Weldment profiles is to put them in a directory separate from the default install directory. Be sure and add that file location to your Weldment Profile file locations (Figure 2). This makes it easy to transfer your custom profiles to a new computer or keep those files when upgrading to a new SOLIDWORKS release so your hard work isn’t lost.
Now that we know the basics, let’s look at two workflows: one to create a profile from scratch and one to edit an existing profile.
Create a Profile from Scratch
To start the first workflow, we’ll edit an existing profile and save as a new name. This is the easiest route if one of the shapes that comes with SOLIDWORKS is what you want, but a simple size dimension needs changing. Within SOLIDWORKS, browse to the default directory mentioned above and open the base shape needed. You’ll notice in the feature tree that the icons for the file are a stack of books and the sketch has an “L” within the sketch icon indicating a library feature is open (Figure 3)
Edit the dimension(s) that need to be changed by editing the sketch (RMB on sketch feature > edit sketch). After the profile is dimensioned as needed, simply save as a new name making sure the file type is still set to SLDFLP. Now you can access that profile size in your dropdown within the Weldments tools structural member command (Figure 4).
Edit an Existing Profile
The second workflow is similar in all the steps except now you start the profile by creating a new part. Sketch out the shape profile needed and add the necessary dimensions. Once the profile has been defined, it is important to note here that SOLIDWORKS uses vertices to locate the Weldment Profile when it is placed. If extra vertices are needed, depending on how the profile will be located, now is a good time to add those to the sketch. This is also a good time to add in a description in the file properties so the cut list will populate correctly when the drawing stage is reached (Figure 5).
Once the profile is established, continue with saving the profile as a Library Feature Part and you’ve just created a custom Weldment Profile.
Another option to take note of that might save some time is to explore the downloadable Weldments content offered in the SOLIDWORKS content folder under the Design Library (Figure 6). There are multiple different Weldment Profiles grouped by standard available within this content.
Within that download folder there are a lot of different shape and size options to explore. For instance, the ANSI Inch download comes with the following profile shapes (Figure 7):
Now that you’ve created some custom profiles or downloaded the library content, you can begin to add structural members to your sketches and create frames and structures quickly and easily.