SolidWorks Tech Tip: Custom Weldment

Crystal Yazvac — Wed, 28 Sep 2011 13:00:27 +0000

It turns out that many SolidWorks users have applied their knowledge of SolidWorks for personal projects. For example: An Ultimate Deck.

The best way to do this in SolidWorks is to make use of Weldments. However, there is some grunt work involved before we can get creative. SolidWorks Weldments has many standard profiles available to you, everything from ANSI Tube (Square) to Unistrut Aluminum. All of these can be added to your library by going to the Design Library tab-> SolidWorks Content->Weldments and CTRL + Click the items you want to download. Unfortunately there is no existing library for Wood members. So, below will be the steps to take to create your own custom Weldment profile.

1. Folder Structure is important.

a. Check the location of your Weldment profiles at Tools->Options->System Options-> File Locations->Weldment Profiles. Mine was found in C:\Program Files\SolidWorks Corp 2011\SolidWorks\data\weldment profiles.

b. Open a Windows Explorer window and browse to the location. There is a folder for each Standard that you have previously installed. Whatever the folder is called is what the Standard in SolidWorks is listed as.

c. Create two new folders, the first one I called “Custom”. Open “Custom” and create a second folder called “Wood”. Any profiles you create for this project will be saved in the “Wood” folder.

2. Create the profile.

a. Create a new part and start a sketch.

b. I started with a 2X4 (which is actually 1.5” x 3.5”)

c. You might also want to add in some extra points in your sketch. This will give you more control of the placement of your profile when adding in the Structural Member.

d. Then go to File->Save As and save the part as a “Lib Feat Part”. Make sure my location is pointed to the “Wood” folder we created in step 1c. The file name should reflect the size, in this case “2X4”.

e. Repeat Steps 2a – 2c for other sizes of wood.

3. Now it is time to create.

a. You will notice when you add your first Structural Member that you now have a Standard option of “Custom” and a “Type” selection of “Wood” and all of your profiles are listed in the “Size” drop down box.

Here is an example of the deck I created in a matter of minutes using my custom Weldment profiles.

Interesting Corner on Welded Frame

Michael LaFleche — Tue, 12 Jan 2010 13:52:23 +0000

Have you ever wanted to have a nice equal mitre cut on the corner of a weldment? This is possible since SolidWorks provides tools to group weldment profiles together in one feature. The try this out yourselves, create a 3DSketch of your frame structure, insert a weldment feature, then insert a structural member. Select the top two consecutive edges in the 3DSketch and choose “Mitre” as the corner treatment option. Then, choose the “New Group” option and select the vertical member. You will notice that the default is the make a flat cut up to the mitered cut above it. This is fine on many weldments. But if there is a special situation where you need an equal mitre cut for rigidity’s sake, you have the option to choose from multiple corner treatment types. While you are still in the structural member setup, you will notice a blue dot on the corner of your weldment preview on your screen. Click the blue dot and you will be presented with a box. Here, change the “Trim Order” from “1″ to “2″ and gawk in amazement! you now have an equal mitre cut!

Download the weldment part here from my 3DContentCentral library.

CAPUniversity » Weldment

SolidWorks Tech Tip: Custom Weldment

Interesting Corner on Welded Frame