Learn how to refine connectors, add a fillet, and clean up your design using Autodesk Fusion 360. This walkthrough guides you through the process of resolving geometry conflicts, creating new sketches, manipulating the extrude tool, and updating your material appearance to result in a clean, complex design.
Key Insights
- The walkthrough starts with refining connectors by adding a fillet and adjusting the radius to 12. This results in the resolution of geometry conflicts within the clamp space.
- The guide then proceeds with the creation of a new sketch using the clamp center, the manipulation of the extrude tool to cut through the left and right support, and the setting of the extrusion distance to 100. This allows visibility through the top clamp.
- Finally, the walkthrough concludes with the construction of an offset plane, the application of the extrude command to cut through the bottom clamp, and the update of the material appearance to plastic matte black. This results in a clean, one-body design, ready for saving.
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Now let's refine these connectors. We'll begin by adding a fillet. We'll go up to our modify area, select fillet, and we want to select our four curved edges.
With all four edges selected, we can change the radius, and we want 12. Look at that result, it looks good. We'll go ahead and click OK.
Now we want to clean up the inside. If we look down inside of our clamp, we'll notice that our connector is conflicting. It's still going through that clamp space.
So let's go ahead and create a new sketch. And we want to use the clamp center. Click on clamp center.
I might have to move back up to that clamp. And we'll go the easy route this time and select our existing geometry. We'll go to create, project, include, project.
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And we have to carefully hover over the very center circle, click one time, and click OK. So there is our sketch. It's right in the center of our clamp.
Now we can select that sketch and do an extrude. So let's first go finish sketch. Look for that extrude tool.
We want to select that sketch, which is currently just called sketch four. Again, we can see it's locked because it is dependent on the geometry. And we'll change our direction to symmetric.
And we'll grab these arrows and pull it all the way out. We'll notice that Fusion is really smart and it starts to cut. Let's double check the objects it's cutting.
We want to make sure it's cutting both the left support and the right support. And we can pull it out any distance. I like to use nice round numbers.
We'll give it a distance of 100 and click OK. So there it is. Now we can see all the way through our clamp on the top.
Now let's go to the bottom. We still have that conflict down there. So let's go ahead and repeat that process.
This time we'll need to create our own construction plane. We'll go to construct menu, we'll do offset plane, and we'll click on the bottom face. So the bottom of that T, we'll click one time.
Now place a construction plane right there at the bottom and we'll click OK. It's called plane three. We'll call it clamp bottom.
Clamp bottom. Now we'll select nothing, begin our create sketch command again, and select clamp bottom. So looking straight up at the bottom of our T, again, we'll go the easy route.
Go to create, go to project, include, project, and we want the inside of this circle. Click one time. And if it's not there, if I orbit, I'll notice there's a sketch right there at the bottom of our T. It's a perfect circle.
And we'll click OK. Now we'll go back to finish sketch, go to the extrude command, and we can drag this one backwards up through our T. And we don't want to go too far because we'd go out the top of our T. Just want to go up about to the center, which is minus 50 exactly. And we want to double check what's getting cut, just our left and right support.
Go ahead and click OK. Now if we double check, we can look up to the bottom and everything is nice and hollow again as it was. But we have a couple of housekeeping items.
First off, these sketches are unnamed. So the first one we'll call this top connector cut. And the other one we'll call it bottom connector cut.
Now we want to have nothing selected at all. We'll click out in blank space. And we want to combine all three of these bodies into one.
Here in the modify area, we notice a combine tool. We'll click combine. So what's the target body? I like to think of the target body as that component of the whatever we're working on that remains.
So that is our target. I want the clamp to remain. So I'll click on the clamp.
And then the tool bodies are the ones that act on the target. We'll click the left and right support. We should have two selected.
The operations should remain as join. And we don't need anything else checked. We're going to go ahead and click OK.
It combines everything into one body called clamp. Nice and clean. Look at that.
Everything looks really good. It got rid of the extra lines. And it's all one body.
Pretty complex body. And all the shapes we created ended up making this one object. Now it's currently set as steel.
We want to update the material. So let's go ahead and click on clamp. Right click.
Go to appearance. And we already have plastic used in our design. We're going to use it again.
So here in the appearance window in this design, we have one called plastic matte black. We'll click and drag it. And I like to drag it right to the project browser, to the bodies folder where it says clamp.
And I'll let go. And that applies that black plastic. All right, that looks pretty good.
I can close my appearance window and minimize my folders. And now I can unhide everything. And we'll activate the top line to see how it looks.
There it is. We now have our handlebar clamp right at the top of our scooter. It's an awesome time to go ahead and click that save icon.
