Discover the process of creating and modifying a metal folding bracket using CAD software, including importing a pre-existing shape, extruding profiles, and employing the fillet tool. Learn how to navigate the complexities of the software to avoid cutting unintended components and how to generate a flat pattern for potential fabrication.
Key Insights
- The article provides a detailed guide on making a metal folding bracket in a CAD program, starting with the insertion of a pre-designed shape using the DXF file format.
- It elaborates on the selection and extrusion of different profiles using CAD software, emphasizing the careful selection of specific components to avoid unintentional modifications.
- The piece concludes by illustrating how to generate a flat pattern for the bracket, indicating the potential for actual fabrication based on the digital model.
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Our metal folding bracket is looking really good. Now we can cut it to create the shape that we're looking for. Let's start by clicking the Home button on our ViewCube and then going to the Construct menu and selecting Offset Plane.
We want to select the plane that's right at the center of our scooter and we will keep the distance at zero millimeters and click OK. That's going to create a new plane. Let's select it in our browser and give it a name.
We'll call this Bracket Center. Now let's assume that the shape we're going to cut into our bracket was already created in another CAD program. All we need to do is import it.
We're going to go up to the Insert and we're going to select Insert DXF. The plane we want to place our DXF onto is this Bracket Center. We will select that first and then we need to pick our DXF file.
This will be a course download. You want to download this file and save it to your computer. The file is called Fusion 101 Folding Bracket Profile.
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Go ahead and open it and we can leave everything alone. All the settings look good. We will just click OK.
There it is and it already has a name because it's a DXF file that came with its own name. We are ready to rock and roll using it for an extrusion. Let's zoom in nice and tight and under the Create menu we want to select Extrude.
Now we can select the profiles in the Extrude menu. Let's start with the smallest profile first. If we zoom in right tight to our sketch there is a circle right in the center.
Now if it's hard to select sometimes we can hold CTRL on our keyboard or we can rotate our view so we're looking to see right at that little circle. It's a little bit tricky to select this guy but if we kind of orbit to get past that flange we can select that little circle. The next shape is this path that the folding takes place on.
I can hold CTRL on my keyboard and click it and that path is selected. Now I can hold CTRL one more time and select the overall outside shape. We want all of the exterior to go away.
Now let's double check everything here. We have our profile plane, the direction set to one side. I want to change that to symmetric and let's go ahead and pull that out visually.
I'm going to pull one side which pulls out both and I want to pull it out far enough that it goes past my flange which ends up being about 30 millimeters. Now we'll notice something else interesting. It's trying to cut but it's cutting many stuff.
You can see it's cutting our wheel, the deck, many things we don't want to cut but there is an option here called objects to cut. If we open that up we can start unchecking geometry. I don't want it to cut the deck so uncheck that.
Uncheck the rail. Uncheck the tire. Uncheck the rim so that the only thing that is checked is my folding bracket.
Once I'm set with that I click okay and there we go. I can see the result. There is that folding bracket and it's looking really good.
The only thing I notice here is that the edges are pretty sharp. How do we fix that? We can use the fillet tool. Under modify we're looking for fillet and I will click all four of these small edges right at the top of our bracket.
One, two, three, four and now I can set the dimension of that radius which is 10. I want 10 millimeters and I'll click okay. That's looking really good.
I've got a really nice folding bracket here. The cool thing about Fusion is that it is loaded with manufacturing technology. In addition to creating this model I can also think about how it is made.
If I go up to the create menu I see a tool called create flat pattern and as long as I'm still working in my folding bracket I can click on create flat pattern. It wants me to select a stationary face. What does that mean? Essentially it's the part of the metal that doesn't move.
I'm going to click right here at the bottom. That portion doesn't fold or bend. Just click right here on the base one time and I'll click okay.
Now Fusion thinks for a moment and creates a flat pattern. This could be cut for example plasma cut out of a sheet of steel and then it shows the bend locations as well so that this could actually be fabricated. All I have to do is click export to DXF and take that over to my plasma cutter and I'm good to go.
For now we will just click the green finish flat pattern check box and it takes us right back to our model. At this point we can click the save button and we are all complete with our folding bracket.
