Weldments

How to create custom weldment profiles in solidworks.

Overview

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.

Benefits of using weldments command

Why would you go through such length to use the weldments command when you can use sweep or extrude instead? Well, like most of the other features in Solidworks the weldment command is aiming to serve specific scenarios, hence the name. Weldment creates a multi-body part that is useful in drawing documents. But, the benefits don’t stop there.

• You can use pre-defined cross sections stored in a library for your organization.
• You can change the length, depth, or width of the structure without changing the profiles.
• You can use cut-list tables in drawings.
• And in simulation environment Solidworks uses correct mesh type out of the box.

Activate weldment tab

The first step in creating weldments in SolidWORKS is accessing the weldment tab. To add the weldment tab to your SolidWORKS graphics area follow these steps.

1. Press Ctrl + N and in the window that appears select Part and then Ok.
2. 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.

Adding weldment cross sections (profiles) to SOLIDWORKS

As I mentioned, to work with weldments in solidworks you need a skeleton and a profile to extrude along that skeleton. In this section I will explain how to use solidworks standard libraries and how to introduce new profiles to the software.

What are cross section files and where are they?

Cross section profiles are sketches saved as .SLDLFP files through a specific procedure. Solidworks uses the points in these sketches to place them on a line or curve and then extrudes them along that path. The process is verys similar to sweep command. However these profiles should be saved in the folder that solidworks knows about and more importantly with the folder structure that solidworks can work with. Weldment profiles in SolidWORKS should have these features:

1. file extension should be .SLDLFP
2. should be closed sketches with at least one contour.
3. Stored in a directory with this folder structure:

SolidWORKS weldment profile folder
\---standard name                           <-- sub-folder
    +---type of profile                     <-- sub-folder  
    |       cross section file name.SLDLFP  <-- file
    |       cross section file name.SLDLFP
    |       cross section file name.SLDLFP

Solidworks will use this folder structure to display profiles in the weldment environment.

Where is the weldment profile folder?

To find the folder to save weldment profiles follow these steps:

1. Next to SolidWORKS logo select Tools > Options.
2. In the window that appears select the System Options tab.
3. From the list on the left select the File Locations.
4. From the SHOW FOLDERS FOR drop down on the top of the window select WELDMENT PROFILES.

This is the folder you should copy the weldment profiles into. Folder structure is important. The default libraries that we will downloaded later are structured properly and should work out of the box. Once downloaded, extract the content into the folder that you found in the steps above. For example I have downloaded the Unistrut library and extracted the .rar file into the WELDMENT PROFILES and this is the folder structure:

C:\PROGRAM FILES\SOLIDWORKS CORP\SOLIDWORKS\LANG\ENGLISH\WELDMENT PROFILES
\---Unistrut                <-- Name of the Standard
    +---Aluminum            <-- Member Family (Type)
    |       40x40.SLDLFP    
    |       A1000.SLDLFP
    |       A4000.SLDLFP
    |       A4001.SLDLFP
    |       P1000.SLDLFP
    |       P1001.SLDLFP
    |       P4000.SLDLFP
    |       P4001.SLDLFP
    |       P5500.SLDLFP
    |       P6000.SLDLFP
    |       P6001.SLDLFP
    |       P7000.SLDLFP
    |       P7001.SLDLFP    <--Cross section files (Size)
    |       
    +---Fiberglass
    |       F1000.SLDLFP
    |       F1001.SLDLFP
    |       F3300.SLDLFP
    |       F3301.SLDLFP
    |       
    +---Steel 114
    |       A1000.SLDLFP
    |       A1001.SLDLFP
    |       
    +---Steel 1316
    |       P6000.SLDLFP
    |       P6001.SLDLFP
    |       
    \---Steel 158
            P1000.SLDLFP
            P1001 3.SLDLFP
            

Solidworks will use this folder structure to fill in the properties in the weldment command as shown below.

How to download a standard library of weldments profiles for SolidWORKS

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.

1. Make sure Task Pane is accessible. From the top, right-click on a tab > Toolbars > Task pane.
2. Click on Design library icon in task pane > expand Solidworks Content > weldments
3. To download a library, hold down Ctrl and click on the library you need.
4. Save the zip files on your desktop.

After downloading the library you should extract it to the Weldment Profile folder.

How to create a custom weldment profile

Although SolidWORKS has a library of standard profiles you might need to create a separate library for your company

1. Open SolidWORKS as administrator
2. Create the cross section of the profile. Keep in mind that the origin of sketch is the default insertion point for the profile. You can use all the sketch points in the profile to locate the profile along the structure skeleton.
3. add a custom property to the file and call it Description. For the value enter the standard followed by type of the profile and its size. this property is important because SolidWORKS will use it in weldment cut lists.
4. Select and highlight the sketch in design tree. If you miss this step you will receive an error message that the library feature is empty when you want to use it.
5. Save the file as lib feat part .SLDLFP in the weldment profile folder. You need to follow the folder structure pattern we discuss in the next section.

Creating wire-frame as skeletons

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.

1. Press Ctrl + N and in the window that appears select a part document
2. Go to Sketch tab and expand sketch command and select 3D sketch
3. Use hot-key L to draw a line in SolidWORKS
4. Pay attention to the plane of this sketch as it appears next to the pointer
5. To change the plane in 3D sketches rotate the model a bit and then use Tab key
6. Keep in mind that you can always use Along x, y and z constraint to further define your sketches

Extruding cross sections (Profiles) along wire-frames

1. make sure you have activated the weldment tab as discussed above
2. make sure you have a skeleton of your design following the steps mentioned above
3. in the weldment tab click on the Structural Member command
4. 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.
5. Choose the standard, then the type of the profile (for example I-beam or pfc) and then the size of that profile.
6. 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.
7. Each group has segments (members) that you select from the graphics area.
8. 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.

Apply Corner treatment

This command allows you to cut the ends of each beam. “Miter” cuts the beams in 45 degrees whilst the other types cut by 90. The trim order defines which group of profiles are the dominant ones. The group with the higher order cuts through the ones with lesser orders. if two groups have the same order numbers then the cut a miter.

Mirror profile

This command mirrors the profile either horizontally or vertically.

Rotation Angle

Allows you to rotate the profile along the line in that specific group.

Conclusion

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 weldmnets 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.

Also see

How to make a sheet for each unique body in a weldment drawing