I like learning about technology and IOT. I also dabble in 3D design and 3D printing.
Planter and Tray Tutorial
While I love working in Solidworks, I cannot get over the intuitive interface Fusion 360 has to offer. In this short tutorial, we'll design a minimalist planter and its tray from scratch. We'll run through sketch tools along with some basic 3D features like the Extrude and Fillet.
Step 1: Start the Sketch
Let's start a new design! Start Fusion 360 and it should open a new (Untitled) file by default. Let’s start a sketch on the XY plane. To do this, click the Create Sketch button (top row, the first button next to Model drop-down). Then click on the XY plane in the work-space.
The view will rearrange, and we’ll begin by drawing a heptagon. Why a heptagon? Because the web is full of planters that are hexagonal or usually ( n <= 6 ) - sided.
Step 2: Draw the Heptagon
How do we draw a heptagon in Fusion 360? Well, in the sketch drop-down, select Polygon. In the new menu that appears, select the Circumscribed Polygon. Click on the origin to place the center. Then start dragging outside. You’ll notice that while dragging, the default shape is a hexagon.
Don’t click to place it yet. While dragging you will also notice two floating inputs. One of them, the radius, is active by default. Drag the shape upwards until you get at about 25 mm.
If Fusion 360 doesn’t snap by default to the grid, you can enable this behavior in the settings. While dragging the shape with the dimension input selected by default, type in 25mm. Don’t hit the Enter key yet. We still need to define the number of edges.
To do this, after you typed the radius (25mm), hit the Tab key to jump to the other available input. Instead of the 6-sided default, type 7, then hit Enter. You should now have a circumscribed heptagon with a radius of 25 mm.
Step 3: Drill Some Holes
Right now we have the base for our planter. We should add some holes as well so the water doesn’t build up at the bottom and cause root rot.
We’ll start by adding a circle inside our heptagon. Select from the Sketch drop-down the Circle tool. Then the Center Diameter Circle (also notice the “C” key shortcut here). The tool works by first placing the center with a click, then the radius with another click.
So place a circle inside the top part of the heptagon anywhere. Next, we’ll make sure to add a vertical relation with the origin.
Step 4: Add Relations and Dimensions
To add the vertical relation, first, deselect the circle tool with the Escape key. Then click on the circle center point, hold down the Shift key and then select the origin point as well.
With both points selected, right-click anywhere to bring up the contextual menu. Select the Horizontal/Vertical option. Now the circle center point and the origin should have a vertical relation.
We should also consider giving the circle a dimension. Click on the sketch drop-down in the menu, then select the Sketch Dimension tool. Also, notice the “D” key shortcut. We will define the diameter of the circle and its distance from the top. With the Sketch Dimension tool active, click the circle perimeter. Now drag out the dimension and click to place it. Input 3mm.
With the Sketch Dimension tool still active, click on the center point of the circle. Then click the top line of the heptagon. Drag the dimension outside of the heptagon. Click to place it. It will ask to input a dimension. Add in 4.5mm then hit Enter.
Step 5: Use the Rectangular Pattern to Create More Circles
Now we’ll create 2 more circles by using the Rectangular Pattern. To do this, click on the sketch drop down, and select Rectangular Pattern. This feature takes in several parameters, but we will use it in a simple way.
First, it asks us for objects for the pattern. Click on the circle we created. Two arrows will appear. Grab the top arrow and drag it down until the Distance input reads -15mm (that's right, negative 15mm). The number of objects to create is by default 3, so leave this alone. Click on OK in the Rectangular Pattern window to apply the pattern.
Step 6: Create a Radial Pattern
Now let’s repeat these 3 circles in a radial fashion. Click on the sketch drop down, then select the Circular Pattern.
This feature requires the Objects and the center point for the radial pattern.
So for our Objects select the three circles. There's no need to hold down the Shift key since you can add many entities to the selection by clicking.
Click on the Center Point input in the Circular Pattern window and select the origin point. A preview will appear with a default of 3 instances of the pattern. You’ll also notice a new field in the Circular Pattern window called Quantity. Input 7 in this field and then hit Enter to apply the pattern.
Step 7: Apply an Extrusion
The sketch is complete! Now we’re ready to apply our first 3D feature, an extrusion.
Click the Stop Sketch at the end of the top toolbar. You’ll notice all the relations and dimensions disappear.
In the Create drop-down, next to the Sketch drop-down select the Extrude feature. For the Profile, click anywhere in the heptagon (but not inside one of the circles). For the Distance field inside the Extrude window, input 3mm then click OK.
Click and drag the cube at the top right to rotate the part a bit and get a better look at it.