We show you how to use the Revolve and Pattern Tools in Fusion 360 to easily create complex circular objects and save time with your CAD designs.

Last month, we provided a basic introduction into Computer Aided Design (CAD) using Fusion 360, including how to install it. This month, we are going to build upon what we learned and introduce you to some more advanced features. In particular, the revolve tool, which we consider to be one of the key Fusion 360 features you should learn.

The revolve tool allows you to easily model complex shapes that are consistent around a single axis. It is perfect for circular shapes with varying dimensions, including wheels, knobs, bushings and bottles, and the jog-wheel from the MIDI controller in this Issue.

In addition, we will look at the Pattern tool which allows us to replicate a drawn or extruded feature along an axis, line or direction, etc. This is an easy way to add recurring details, and is a very powerful tool you will likely use all the time.

ACCURATE MEASUREMENTS FOR CAD

In Part 1, we designed a radius gauge from scratch using the drawing tools and some mathematics. In this tutorial, we will design a 3D model based on a real-world object that we can physically measure. For accurate measurements, we will use a Digital Vernier Caliper. This is a handy tool to have in your toolbox, and perfect for CAD modelling when you have the part you wish to model in your hand. You can pick them up from electronics stores from as little as $14.

Parts / Tools Required:	Jaycar
1 x Digital Vernier Calipers	TD2081
1 x 18mm Dia. D Shart Plastic Knob	HK7709

There are three common ways to use a caliper to take measurements:

• Outside jaw to measure the external diameter of an object
• Inside jaw to measure the internal diameter of an object
• Depth probe to measure, as the name suggests, the depth of an internal hole

THE REVOLVE TOOL

Since many projects in a maker’s life use potentiometers, we thought designing and printing our own 3D knobs was a great way to learn how to model round objects in CAD.

Before we begin, we need to get hold of a knob to model. For our tutorial, we chose the HK7709 push on style knob from Jaycar, but it appears the H6022 from Altronics is the same.

The revolve tool in Fusion 360 means we only need to draw one half of the profile because the revolve tool will revolve the device 360° around our desired axis. Let’s demonstrate.

Start by loading up Fusion 360 and create a new design.

Press ‘L’ on your keyboard to toggle the line tool. Simply draw the general outline of the knob’s profile, as we show you here. We don’t need to worry about dimensions in this step.

Press ‘D’ on the keyboard and start to enter the dimensions, being careful to work from the smallest diameter to the largest on each plane, which prevents the model essentially turning itself inside out.

Use your Vernier calipers to measure the topmost diameter of the knob. Ours measures 13.62mm in diameter. To enter this value simply click on the relevant line in the sketch and enter ‘13.62/2’. This will add the correct radius dimension to the top of the sketch.

Next, carefully measure the other dimensions and add their values to the sketch. You may find it easier to set the lower dimension (above the taper) by first drawing a line from the centre line 7.965mm, or half of the required diameter, and using this as your reference. Take your time to verify the dimensions are correct. Once you’re done it should look similar to this.

We must also consider that our end goal here is to 3D print the object, so we will need to modify the design slightly to assist in this printing process. For example, we need to remove the overhangs, which we show you in this image.

This will allow us to print it upside down, without needing to use extra material to support this overhang. This will help reduce the time taken to print, and also improve the appearance of the finished object.

Once you’re positive the dimensions are correct and satisfied with the shape we need to enter a centreline, which will work as the axis point we want the drawing to revolve around. To do this, click on the Construct dropdown arrow and select ‘Axis through edge’.

You then want to select the right edge and press Enter. This will create a construction line which defines that edge as a CentrePoint. We next want to revolve the feature around this point. This is done by clicking the create dropdown arrow and clicking revolve.

You want to select the sections to revolve by clicking on them. Next, click the axis selection box and choose the construction line you just made.

The type dropdown allows you to choose between Full, Angle and To:

FULL: Extrude the sketch around a full 360°

ANGLE: Allows you to select any angle between 0 and 360°

TO: Allows you to extrude it up to another intersecting object

We want to select Full and have it extrude as a new body. This will provide us with the general shape of the knob. We still need to add knurling and, of course, a way to mount it.

The knurling is effectively a way for the user to get grip on the knob so it is easier to turn. On our knob, it is a very simple vertical band which should be easy to replicate. Our first step is to carefully measure the width and depth of the indentation. Using the inside jaw of our Vernier calipers, we were able to measure the width of 1mm. Similarly, using the depth probe, we measured the depth to just 330 microns. This is likely too small for the 3D printer to replicate reliably so we will increase this to 0.5mm.

To draw the knurling, simply press ‘L’ on your keyboard to use the line tool and add a 0.5mm line at the bottom and top of the knob.

You then need to join these lines together following the contour of the knob's angular surface. Once you’re done click the stop sketch button in the ribbon.

We now want to extrude this as a cut, following the previously made centreline. To do this, select the dropdown arrow on the create button in the menu and choose Revolve. Select the body we just drew and pick the construction centreline. Select the type dropdown and choose Angle. We want it to extrude 5° in a symmetric direction and the cut operation.

Our knob has eight of these small indentations so rather than repeating this function seven more times we are going to use the Pattern tool. Click on the create dropdown in the menu, mouse down to Pattern and select the Circular pattern.

You want to select all three of the faces that make up the indent and again select the centreline/construction line we created earlier as the axis. Under type, you want to select Full so the pattern is repeated over the full 360°, and finally set the quantity to 8 so it is repeated eight times.

To finish this feature, we want to add a small chamfer to the inside of these indents, which will minimise overhangs so that it will print without needing supports. Select the modify dropdown arrow from the menu and select Chamfer.

You want to select the internal corner of the indent we just made on all 8 of the indents. Make sure it’s set to equal distance and set the distance to 0.45mm or as large as it will let you.

You will see that the knob is starting to take shape, so now is the time to concentrate on the mounting structure. The first step will be to hollow out the internal structure. To do this, select the modify dropdown arrow in the menu and select Shell.

Select the bottom surface as your face and set the internal thickness to a multiple of at least three times your printer’s nozzle diameter. In our case, this would be (3x0.4), however, we are going to give it a little more thickness and choose four times our nozzle diameter.

With that set, we can start to model the internal structure of the mounting. We recommend using the shaft of the switch or potentiometer the knob is designed to fit. This is much easier than getting your Vernier calipers into the tight spaces of the knob. If you don’t have the switch or potentiometer you can still measure inside the knob with the calipers though. Just take a little more time to make sure the dimensions are correct.

For our knob, the internal dimension for the mount is 6.5mm. We need to add a little more to account for the tolerance of the 3D printer. Depending on your printer, you may need to set it at about 0.25mm larger than what we measure. In this case, 6.75mm.

Press ‘C’ on your keyboard to select the circle drawing tool. Draw a 6.75mm circle with the origin point in the centre of the structure. You then want to create a second circle with the same dimension + (3 x your nozzle diameter). You can enter ‘6.75+(3*0.4)’ if you have a 0.4mm nozzle.

We now want to add the key to this circle so that it locks against the shaft of the switch. Measure the internal diameter of the flat key area across (We measured 5.55mm on ours). Using the line tool, make a vertical line across the circles we just made. Once you’re done it should look like this.

Press ‘E’ to select the Extrude option and extrude the mounting section you just drew.

Select the three main sections of that feature and extrude it out toward the bottom. Using the depth gauge, we can see the knob is 16.5mm deep and the extrusion extrudes to 5mm from the bottom, which means the extrusion is 16.5 – 5mm long. Therefore, in distance, we want to add this number.

You may notice that the internal mounting structure does not really have much in the way of support. This is fine for injection moulded parts, however, we are producing our knob with a 3D printer instead. The 3D manufacturing process has weaknesses due to the layer by layer manufacturing process, coupled with layer adhesion issues. for this reason, we need to deviate slightly from the knob we are modelling.

If we were to simply replicate this design, the knob will likely shear at the join between the centre mounting structure and the knob itself when the user tries to actuate the switch. Instead, we need to create an internal elements to help strengthen the mounting structure. We can easily do this using the revolve and pattern tools we have already used.

To make it easier to visualise the new drawing, we need to create a cross section and split the model in half. Note that this is only a visual tool and does not alter the actual model.

To create the cross-sectional view you need to select the inspect dropdown arrow in the menu and choose Section Analysis.

You need to make sure that Origin lightbulb in the left menu is highlighted as this will enable you to select the plane you want to work from. Since we want to completely cut the model in half, top to bottom, select the vertical planar face as the face for the sectional analysis and click OK.

Press ‘L’ on your keyboard to enter the line drawing tool and trace around the existing gap between the mounting structure and the outer shell of the knob.

Once your shape is drawn, simply select stop sketch from the menu. Next, extrude this shape around the centre construction line axis by selecting the create dropdown arrow and choosing Revolve.

Select the drawing we just made as the profile and the centre construction line as the axis. We want to select angle as the type and set to 20° (you can make this whatever you like but 20° should be fine).

Set the direction as symmetric so it extrudes either side of our drawing equally. Make sure the operation is a new body so that it does not connect this new body to the existing body. Once you’re happy with the results click OK. Note: you can now disable the cutaway view by selecting the highlighted lightbulb on the left menu for analysis.

Use the pattern tool to make this pattern repeat itself along that axis, creating symmetrical supporting structures. Select the create dropdown arrow, mouse down to Pattern and again select the Circular pattern option.

Select the new body we just made as the object and the centre or construction line as the axis. For type, select Full and set the quantity to 3 or more. This will replicate the new body equal distances apart. The three support structures joining the inner mounting structure to the outer shell will significantly increase the strength of the part.

We are now very close to completion. We need to just add an indent to the top of the knob to show its position and create a few chamfers to aid in printability and appearance.

To create the indicator on top of the knob we need to know what angle the knob will sit on the keyed shaft. The knob we are modelling has a coloured cap that can be removed and repositioned as desired. Whilst it’s possible to replicate this in Fusion 360, for the sake of brevity, we will leave it out and just model a fixed position. You can change this position in your design to suit your needs.

We are going to use the flat keyed area of the mounting feature as our reference to create the indent, and first, draw a line from the bottom to coincide with that feature. This way, when you’re looking from the top down, you know where that keyed section is and can use it as a reference for the desired angle.

We have simply drawn a 3.5mm long 1mm wide rectangle using the line tool, which you can select by pressing ‘L’ on your keyboard.

Press the stop sketch button in the menu and extrude the feature using the Push-pull tool, which you can toggle by pressing ‘Q’ on your keyboard.

Select the new drawing as your profile and drag the arrow so it pulls into the feature, creating a 0.5mm indent. Once you’re happy with the results click OK.

Before we finish modelling the knob we will add some chamfers to improve the appearance and, in some cases, ease printing. Click the dropdown arrow on the Modify button in the menu and select the Chamfer tool. You want to apply a small chamfer of 0.5mm to the bottom sections of the knob to give them a nice finish. You may also want to the top edges of the knob a 0.4mm chamfer just for appearance' sake.

When you’re done, select everything by left-clicking and dragging a box over the entire model. Merge the entire model into one piece by using the Combine tool. Enter this mode by clicking the dropdown arrow on the Modify button in the menu and select combine. Make sure everything is selected and the operation is set to join and press the OK button. Your design should now be a single solid object without gaps, holes or non-uniform joins in the mesh.

The final step is to export the design as an .stl file so we can slice it and send it to the printer. Simply select the Make button from the menu to see the 3D print menu. Right-click and hold the mouse button and drag over the entire model to ensure everything is selected. Make sure the refinement is set to High and that ‘Send to 3D printing utility’ checkbox is unchecked.

Give your part a name and tell it what location you wish to save it to.

You can now slice it with your favourite slicer and print as normal. If you find that some of the tolerances were not perfect, too loose or too tight on the shaft, for example, you can simply use the timeline at the bottom left of the screen to go back to the creation of that feature and modify it. Simply right-click the feature you want to modify and select Edit. This will allow you to edit the sketch, feature or action without changing the rest of the model.

PART 1 - BEGINNERS GUIDE TO FUSION 360

PART 3 - BLENDING AND SWEEPING

PART 4 - RENDERING TECHNIQUES

PART 5 - HELICAL SWEEP

PART 6 - IMPROVING MODEL STRENGTH