Strengthening Your Handlebar Clamp by Adding Side Connectors and Support Geometry

Creating Side Supports with Sketching and Extrusion Techniques

Discover the process of strengthening a T-shape handlebar clamp through the addition of side connectors. This detailed guide will take you through the steps of enhancing your clamp design using Fusion for a more robust result.

Key Insights:

  • The article explains in-depth how to add side connectors to a T-shape handlebar clamp to increase its strength. The process involves activating the clamp component, creating a construction plane, and drawing a support sketch.
  • Creating an additional construction plane is necessary for adding the side connectors. The plane is created by selecting three points: two end points of a blue line from the Vertical Tube Sketch and a point on the tube.
  • The article further illustrates how to sketch the support shape using the line tool and the Tangent Arc tool in Fusion. The sketched shape is then mirrored across to avoid redrawing. Finally, the Extrude command is used to convert the sketched profile into 3D geometry.

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Now that we have the T-shape modeled for our handlebar clamp, let's make it even stronger by adding some side connectors. Let's first zoom right into that clamp. We have the T-shape, the vertical portion, and the horizontal portion, and we'll add a couple of connectors or supports on either side.

Step one is to go to our clamp in our project browser and click Activate Component. Then we will hide everything else. This will let us see only the clamp for now.

With that clamp visible and activated, I want to click the little arrow to expand all of its folders. And I want to expand the Sketches folder, and I want to select the Clamp Vertical Tube Sketch and unhide it. We see that sketch coming through here.

Now we need to create another construction plane. Let's go to Construct menu, and we want to select one we haven't used before. It's the plane through three points.

We'll click that. Now we need to select three points per its name. We want to orbit our view until we're looking up a bit from the bottom.

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Now this can be tricky to select, so I'll show you two ways to do it. The first is to select the two end points of the blue line from our Vertical Tube Sketch, and then move to the right and look for a point on our tube. Sometimes we have to orbit around to find it, and there's one, that little white dot.

And with those three points, Fusion makes a plane. Now if that doesn't work for you, I'll show you another way to do it. Instead of starting with the sketch, start with the little points that we find on that vertical tube.

So one on the right, two on the right. So there are two points there, and then we can click the top of our blue line, and that will also create that plane. Now if we orbit around, we should notice that that plane goes right down the center of our clamp, and that's right where we want it.

Once we're happy with it, we'll go ahead and click OK. Now let's hide our Vertical Tube Sketch for now. We don't need to see that, and we'll expand our Construction folder, and we'll see this generic plane.

Let's give it a name, and this time we'll call it Clamp Supports. And with that, let's click out into space so nothing's selected, and we're going to now draw the sketch of our support shape. So let's go up to the Create menu and click on Create Sketch.

We'll create the sketch by first clicking that Clamp Supports plane, and that will reorient our view. We might have to zoom up to the top, and now we're looking directly at our clamp. Now we need some help drawing this sketch.

Right now there isn't much here, just that 3D geometry. We're going to go to that Create menu and look for Project Include and find Project. We will select the Horizontal Tube here first, and then the Vertical Tube, and then click the OK button.

That will set us up with some purple points and lines that will help us sketch. Now we can go to that regular line tool, and we'll start at the bottom purple point, bottom left. We'll click one time and go straight up 8 millimeters, so 8 and Enter.

We'll start the line command again, this time go to that far left purple point, click, and move our cursor to the right. Make sure it's exactly to the right, and then go 8, Enter. Two lines, both 8 millimeters long.

Now we can go to the Create menu, and we're looking for Curve, and it's in Fusion here called Arc, and then Tangent Arc. So Create Arc, Tangent Arc. We'll start at the top of that bottom 8 millimeter line, click one time.

We can see Fusion right away creates a Tangent Arc or Curve, and then click the end point of the other 8 millimeter line. There we go. We can start to see visually that connector.

It's that nice Tangent Arc. But now we need to create the full profile, and we'll draw some lines on the inside. We'll go back to our line tool.

We'll click at that first part of the arc. We'll click one time, go to the right, type in 8, Enter. Now we'll draw another 8 millimeter line from the top of the arc, click, go straight up, type in 8, Enter.

Now we'll create some additional lines right where we left off, and these are more arbitrary. We'll just go straight to the right. We want to make sure we see that perpendicular or 90 degrees, or zero degrees in this case, letting us know we're drawing a straight line.

We'll type in 50, Enter, and we'll start the line command again. Do the same thing from that bottom point, go straight up arbitrarily, make sure it says 90 degrees, and we have that perpendicular constraint. We'll type in 50, and Enter.

Okay, that is our profile. We can even click on it, it turns blue, and we can see the profile. Now let's do a little bit of housekeeping before moving on.

We'll select this first 8 millimeter line, right-click, and go to Normal Construction, make it a construction line. Now this other 8 millimeter line, we'll select it, right-click, and go to Normal Construction. And now we're going to go up to our Modify and select Trim.

We don't need the extra portions of our 50 millimeter line, so we'll click, we'll hover over, and they should turn red on the portions we don't need. We'll click, and they're gone. We just have our profile.

Now we need to create an additional line. We'll go back to our line command, and we're looking for the midpoint at the bottom of our T. We'll click one time and go straight down, let's go about 20, and click Enter. Now this line is simply here to help us mirror the shape across instead of redrawing it.

We'll select that line, right-click, and change that to a center line. Now we want the Mirror command under the Create panel, Mirror. We'll select our objects, which is every portion here of that profile, and the Mirror line, if it wasn't selected already, is that center line.

And we'll click OK. Now we have two profiles, one side and the other. If everything looks good, we'll go ahead and click the Finish Sketch.

So there is our sketch, and we'll see it's a little bit different. It's got a lock, it's got a lot more constraints, and it's pulling from the other geometry in this component. Let's go ahead and select it one time and give it a name.

We'll call this Connector Profile, and there it is. We've the Extrude command to pull this into 3D geometry. So in the Create menu, we can select Extrude.

We can select our profiles visually, so the left side and the right side. We might want to orbit into more of a 3D view, and we can change our direction from one side to symmetric, and we'll start pulling that out. And we'll try a distance of 12.

See if that looks okay. That's looking pretty good, minus the fact that it is cutting. So let's change our operation to New Body.

New Body, and that looks pretty good. We can see it's tangent at two points. It's not going too far past each tube.

We'll go ahead and click OK. That looks good. Now let's open up our bodies, and we'll see that we have Body 3 and Body 4. Body 3 we can call it Left Support, and Body 4 we'll call it Right Support.

Now these names are fairly temporary, because in our next step, these will get absorbed into the main clamp. But for now, it's a great time to go ahead and click the Save button.

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Reid Johnson

Licensed Architect | Contractor | CAD/BIM Specialist

Reid isn't just someone who knows CAD and BIM; he's a licensed architect and contractor who deeply integrates these technologies into every facet of his career. His hands-on experience as a practitioner building real-world projects provides him with an invaluable understanding of how BIM and CAD streamline workflows and enhance design. This practical foundation led him to Autodesk, where he shared his expertise, helping others effectively leverage these powerful tools. Throughout his professional journey, Reid also dedicates himself to education, consistently teaching university courses and shaping the next generation of design professionals by equipping them with essential CAD skills. His unique blend of practical experience, industry knowledge gained at Autodesk, and passion for teaching positions Reid as a true specialist in BIM and CAD technology, capable of bridging the gap between theory and real-world application.

Credentials:

  • Autodesk Fusion Certified User
  • Autodesk Revit Certified Professional
  • Autodesk Certified Instructor
  • Licensed Architect
  • Licensed General Contractor

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