NEWS & ARTICLES

Weldment Assembly Hybrid Drawing

If you are like me, weldments in SOLIDWORKS always seemed like a great idea, but they were always missing some piece of functionality that would make them useful in your company’s workflow. One of the most significant problems that I ran into was mixing in purchased or pre-existing components. Because weldments are a part file, bringing in outside components always required using non-assembly functionality to make it behave more like an assembly.

A better way to achieve this might be to mix using a weldment part with an assembly. But, how do I make the drawing bill of materials look how I need it to? Well, let me show you!

First, we will create a weldment part. I’ll make a very simple one, like so:

Now suppose that I want to add a standard foot pad to this weldment. Of course I could model it in this weldment part, but it’s a standard part, I should use the one in my library! So, I can make an assembly using the weldment part from above and inserting the standard foot pad, like this:

Now I’ve got the weldment that I actually want. I’ve gotten to use the weldment features to create the structural part, miters and all, and I’ve included the standard foot pad that I want.

However, what will my drawing look like? By default, this is what I get in my BOM:

That gets the foot part right, but doesn’t give me the cut list properties I want for the weldment. How do I deal with that?

Here’s how: first, we need a detailed cut list for our assembly BOM. To do this, start creating the assembly BOM like usual, but pay attention to the Property Manager while doing it. Specifically, we need to set the BOM Type to Indented and check the Detailed cut list checkbox, as shown below.

When you click OK, you will get a BOM that looks like this:

This seems to get us a little closer, but maybe I don’t want the weldment part to show, just the pieces. Also, I probably don’t want the cut list information for the foot, as that information is part of the drawing for that part. So, let’s take a look at some other capabilities.

If you hover over the BOM, you will see these arrows show up:

If we click on them, we will see some additional information about our BOM.

The first thing that we can do is collapse the foot part by clicking the – next to it. This will change our BOM so that there is no cut list information for the foot part.

Next, we want to right-click on the weldment symbol next to the weldment part and select Dissolve.

Now our BOM looks like this:

Now we’re close! One of the nice features of a weldment is the ability to show information about the pieces, i.e. length. This is easy, we just need to add that column to our BOM! Right click on the D heading and select Insert->Column Right.

Which will pop up this dialogue box:

Now we just select Length from the Property name drop down list. That gives us the column that we want. Now we can add balloons to our drawing like we would in any assembly, and the customer can’t even tell that we used two different types of modeling to accomplish it.

Of course, all of the information in that BOM can be customized, and you can add columns for raw material identifiers or any other properties. You can also add weld symbols to the appropriate locations and detail each component however you need to. This method just gives you another way to design your weldments.

Making your design projects less cumbersome,

Karl W.
Application Engineer
support@qintegration.com