SolidWORKS weldment is a powerful tool for structural design. combined with other features, it provides flexibility and ease of use to the designer. Its simplicity makes it easy to customize and understand. The core idea is that cross sections will extrude along a wire frame to create a 3d model of the structure. Designers create multi-body parts by using library profiles. Solidworks has a set of libraries for standard structural sections. But designers can add their own sets to the library as well. In this SolidWORKS tutorial we will lean how to use SolidWORKS weldment profiles.
Weldment creates a multi-body part that is useful in drawing documents. But, the benefits don’t stop there.
To add the weldment tab to your SolidWORKS graphics area follow these steps.
Ctrl + N and in the window that appears select
Part and then
Right-click on the part name on top of the window and then press
Tabs followed by
Weldments (make sure weldments is checked)
At this stage all the commands in Weldment tab are grayed out. This is because you need to create a wire-frame. But first things first, let’s see how we can define and import a cross-section.
In this section I will explain how to use solidworks standard libraries and how to introduce new profiles to the software.
Cross section profiles are sketches saved as
.SLDLFP files. You can use them in the Weldment command.
They should have these properties:
To find the folder to save weldment profiles into follow these steps:
This is the folder you should copy the weldment profiles into. Folder structure is important.
The Weldment command has three drop down menus.
These are mapped to the content in the Weldment Profile Folder. As shown below.
The preceding image shows how drop downs in the weldment command are mapped to the files and sub-folders in the Weldment Profile Folder.
Solidworks has a library of standard structural sections. But this library does not ship with the software itself. Users should download this library using the steps below.
Once downloaded, extract the content into the
. For example I have downloaded the Unistrut library and extracted the
.rar file into the
WELDMENT PROFILES and this is the folder structure:
📁---Unistrut <-- Name of the (Standard)
📁---Aluminum <-- Member Family (Type)
| 40x40.SLDLFP <--Cross section files (Size)
Although SolidWORKS has a library of standard profiles you might need to create a separate library for your company
.SLDLFP extension. Otherwise ,when inserting the profile, you will get an error that the library feature is empty.
.SLDLFP in the weldment profile folder.
This youtube video explains the steps in this section. You might find it helpful.
As discussed earlier, weldments profiles are closed sketches that get extruded along another sketch. The latter is a skeleton or wire frame. You need to create the skeleton using 2d or 3d sketches. In this tutorial we will use 3d sketch as it offers better control over the final design result.
Ctrl + N and in the window that appears select a part document
Along x, y and z constraint to further define your sketches
If you want to learn more about 3d sketches you can watch this video.
make sure you have activated the weldment tab as discussed above
make sure you have a skeleton of your design following the steps mentioned above.
in the weldment tab click on the Structural Member command
in the property manager tab that appears on the left select the type of the profile you want. Keep in mind that you cannot choose more than one profile per “Structural Member” command. For example, if you need both I-beams and PFC in the same file then you should run this command once for each type.
Choose the standard, then the type of the profile (for example I-beam or pfc) and then the size of that profile.
Next you should define the groups. “Groups” in SolidWORKS weldment are lines that have at least one shared point. For example, a rectangle is a group of four segments. but parallel lines cannot be members of the same group. so, you need to create a new group for each line.
Each group has segments (members) that you select from the graphics area.
Once you define first group you will get access to more commands inside the property manager.
There are some commands in the property manager that you can use to further edit your design. Below are some of these commands.
This checkbox allows you to cut the ends of each beam. You can define weldment gaps or
Allow protrusion. The trim order defines which group of profiles are the dominant ones.
This command mirrors the profile either horizontally or vertically.
Allows you to rotate the profile along the line in that specific group.
We discussed how you can create a weldment profile and how you should use it in SolidWORKS. We cover all the important features and tips and tricks related to weldments in solidwroks. However, there is always more to learn. You can use links below to learn more about SolidWORKS weldment profiles and how to use them.
Making a sheet for each body in a weldment drawing I