From the course: Fusion 360: Design a Parametric Standing Desk

Designing the support bar - Fusion 360 Tutorial

From the course: Fusion 360: Design a Parametric Standing Desk

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Designing the support bar

- [Instructor] To get started with our first support bar, we will need to create a new component. Remember, components will keep our sketches, bodies, and other assets grouped according to each part. Creating components is required to assemble parts with Fusion 360's Joint command. We can name this component Support Bar. Double-check that your top-level component is active. Otherwise, the component will be nested underneath a different component. If not, you can clear the parent selector and click on the top-level component before clicking OK. Hiding the side panel components will ensure they are not in the way as we sketch the support bar. We'll use joints to position this part so it does not matter which origin plane we sketch on. With the two-point rectangle tool, sketch out a rectangle that starts from the origin point. Remember starting from each component's origin point will ensure the sketch is constrained and not floating in space. Let's add a dimension to the width of the bar. This support bar needs to be wider than our side panels so the material can connect to each slot. Thus, we can type out the width parameter plus an additional three and a half inches, leaving us with an inch on each side, not counting the plywood thickness. The height of our support bar will be four inches. If you recall, we made the slots two inches deep. We'll eventually cut the same two slots in the support bar. So we want this to be twice the size. To reduce waste of material, we can cut away some excess in the bottom center of this bar. Let's hit the Escape key to clear all commands and right-click and delete the bottom line. I'll sketch a straight line and an angled line that heads toward the center, along with the same shape on the opposite side. We want this shape to remain symmetrical. This is a great use case of the symmetry constraint. Let's first create a construction line down the middle, ensuring it starts from the midpoint constraint where the triangle icon appears. Applying a vertical constraint will force the line to remain vertical. We can now select the bottom two lines with a symmetry constraint, followed by the middle construction line. This construction line was required to serve as the symmetry line. Repeat the process for the angled line. Notice how the symmetry constraint keeps the geometry symmetrical on each side of the construction line. Dimension one of the bottom lines with two and a half inches, ensuring we have sufficient room for the slot cutouts. At this point, our sketch needs one additional dimension to become fully defined. Let's dimension the middle line. To keep the sketch driven by the overall height, we can select the four-inch dimension. Notice how that places the dimension number in the input. This allows us to reference the value of existing dimensions. Divide the number by two and click Enter. Our sketch should now be fully defined. We completed the support bar with consideration to minimizing the material needed. Let's extrude this to the plywood thickness parameter. Our support bar is now complete and we can turn the side panel components back on in the browser. We're now ready to use joints to move the part into place.

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