Weldments is one of my favorite parts of SOLIDWORKS. If you are unfamiliar with what a weldment part is, it’s a feature in SOLIDWORKS used to create models that consist of members. It’s a fantastic way to be able to create cut lists directly from your solid model. With the Structure System being introduced a few years ago, creating these structures is easier than ever.
Because weldments can be taken advantage of in many different industries, we need the flexibility to change what shape the members we are going to create are. Let’s walk through the steps required to get these members customized.
Step 1: Find where your Weldment templates are saved
To find where SOLIDWORKS is going to go looking for our templates, we need to look at where our File Location option is pointing to. To find this, go into your System Options, then File Location, use the drop-down to go to Weldment Profiles, and you should see the location listed in the Folders section.
The default location is install_dir\data\weldment profiles
Sometimes, depending on your I.T. department’s security settings, you may not be able to access or edit this folder, so I am going to show you how to add a new customized folder. I have created a new folder called “Weldment Profiles” in my C drive and added this to my system options for my Weldment Profiles.
Step 2: Create your folder structure
This is the part where I find some of my users have the most confusion. When creating a Structural Member, SOLIDWORKS is going to ask you for three things: Standard, Type, and Size. So, because of this, we need three folders: home, standard, and types.
The Home folder will contain folders for all different types of Standards that you need (for example ANSI and ISO folders). This is where you point your System Options to.
The Standard folders will then house folders for different Types of members (for example, c channel, pipes, planks).
Then finally inside the Type folders we will save our files which will be the sizes we need to pick.
The structure should look like this:
Type folders will house .sldlfp files. (see Step 4)
Step 3: Create your custom shape
Create a sketch of what you want your member to look like. For this example, I am going to create a simple rectangle to represent a 2 x 4 Plank.
Step 4: Save as a Library Feature Part
If we just save this as a standard .sldprt file, SOLIDWORKS will not understand this is a template. We need to save this as a Lib Feat Part (.sldlfp). This Library Feature Part file type is a little different from saving a normal part file, and we need to make sure that our sketch is recognized as a reference.
IF YOU SKIP THIS STEP YOUR TEMPLATE WILL NOT WORK.
Before you hit save as, HIGHLIGHT your sketch. Then Save As, Lib Feat Part, and save this into your chosen type folder.
Your part design tree should look a little different when this is saved. Notice the part icon is now library books and we have some new folders at the top of the tree.
I am now able to use customized profiles.
If you would like to learn more about Weldments, join us in one of our Weldments classes where we talk all things structures. Or if you are interested in learning more about Lib Feat Parts, check out our advanced part modeling class where we should you how to create other custom templates for different features like threads.
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