Fusion 360: Using Nubs and Indentations to Attach a Case’s Cover

Introduction

I have watched several videos to learn Autodesk Fusion 360, and to find out how to create nubs and indentations. All the videos were very well down. I learned a lot from them. Two things bothered me. It was hard to grasp all the details without having to frequently stop the video, and rewind it, to view important missed instructions. The second thing was that I wanted to create a list of steps to practice creating models several times. Creating a list of steps by hand was time consuming and subject to errors.

I decided to try another approach, i.e. creating a Fusion 360 tutorial as a list of steps and screen captures. Such a tutorial could be used to quickly practice building a model several times. This enabled the rehersal of fundamental Fusion 360 commands. Your suggestions on how to improve non-video tutorials are welcome.

Overview

To enable a snap-on cover, you can put nubs on a case’s inside faces, and corresponding indentations on its cover’s lip. This results in a tightly fitting cover that will not come off easily. We will detail the steps to do this for a simple enclosure using Fusion 360. First an overview of some details.

The sides of the case will be 1 mm thick. The nubs will be made by creating a 2 x 10 mm rectangle centered on an inside face of the case’s side. The rectangle will be extruded 1 mm towards the center of the case, be positioned colinear with the top edge of the face, and chamfered to form a triangular shape. Here is what a nub looks like.

We began to make the cover by selecting the top surface of the case’s sides. A Sketch was used to create a 1.1 mm offset from the inner edge of this top surface. This area will be used for the thickness of the cover’s lip (1.0 mm) and a small (0.1 mm) clearance for the lip. The cover was made by selecting the 3 faces that comprise the case’s top, and doing an extrusion of 1 mm with the operation set to new body.

The cover’s lip was made by selecting the offset area and doing an extrusion of -2 mm. Clearance for the cover was done using the Press and Pull command to change the lip’s thickness from 1.1 to 1.0 mm.

Suppport material was added to the lip’s inside faces in back of the indentations.

The indentations were placed on the short sides of the lip that correspond to a nub. They were made by drawing a 2 x 10.0 mm rectangle centered on an outside face of the cover’s lip. The rectangle was extruded -1 mm towards the center of the case and made colinear with the top edge of the lip’s face.

Using Fusion 360

Creating the Case

Open Fusion 360 and click on the Create Sketch icon. Move your mouse and select the xy plane as shown below.

After selecting the plane, Fusion changes to the TOP view.

Press R for a 2-point rectangle. Choose 0,0 for the first point and move the move the mouse to generate the rectangle’s width and height. Make the width 40 mm and press tab to make the height 30 mm. Now press return.

Press the STOP SKETCH icon (in the Toolbar). Fusion changes to the Home view as shown below.

Press E for extrude and select your rectangle.

Type in 15 mm for the distance to extrude. Make sure Operation is set to New Body. Press return.

Expand the Bodies folder in the BROWSER to see the new body. You can select it by clicking on Body 1 in the BROWSER.

Now we will shell out body1. Select its top by clicking on it. Press S to bring up the Model Toolbox. Type in sh and select the Shell command.

Fusion 360 is now asking for the thickness of the shell’s sides. Make it 1 mm.

Press OK and the case appears.

Creating the Nubs

We will create two nubs, one on each of the case’s short sides.

Select the inside of a short side and click the Create Sketch icon. Fusion 360 shows the face that you selected in a 2D view.

From the SKETCH-dropdown-menu choose Rectangle and then Center Rectangle. Move the mouse along the top edge of the face until a triangle appears. The triangle indicates the center of the edge. Move the mouse down and then click to set the center of the rectangle. Now drag the mouse and enter its height (2 mm) and its width (10 mm). Press return.

In the SKETCH PALETTE, click on the Colinear icon. Select the top edge of the 2 by 10 rectangle and then the top edge of the side’s face. Fusion 360 moves the rectangle so its top edge is colinear to the top edge of the face.

Press the STOP SKETCH icon. Go to the HOME view. Press E for the EXTRUDE command and select the 2 by 10 rectangle. Set the distance to 1 mm.

Press OK.

Now we will Chamfer the nub. Press S to bring up the Model Toolbox. Type in ch and choose Chamfer. Select the top edge of the nub and then the bottom edge. Type in 1 mm for the Distance and press OK.

Select the opposite side of the box. Follow the above to create a nub on it.

Creating the Cover

We will use the top surface of the case’s sides to create the cover. I needed to zoom-in to select the top surface of the sides. Here is what the selection should look like.

Click on the Create Sketch icon to create a new sketch. In the BROWSER, name the new sketch Cover. Fusion 360 changes to the TOP-2D view. Change to the Home view by clicking on the small small icon that is part of the View-cube at the upper-right of the screen.

We want to make an offset. You can type the letter O shortcut. Select the inside edge and type in 1.1 for the Offset position. Press OK. It should look like this.

Press the STOP SKETCH icon. Press E to Extrude. Select 3 things 1) the top of the walls, 2) the area between the top of the wall and the offset, and 3) the top surface. It should like similar to this.

Set the distance to 1 mm. Change the Operation to New Body. Press OK.

The cover has been created as Body2. In the BROWSER change the name of Body1 to Case and Body2 to Cover. The BWOWSER should look similar to the following.

You can toggle the visibility of the Case and Cover by clicking on their light bulb. Hide the Case.

Making the Cover’s Lip

We will work with the cover upside down. I flipped it by clicking and dragging on the View-cube at the top-right of the screen. Click on the FRONT-RIGHT edge and drag up. Then click on the BOTTOM side of the View-cube. Click the lightbulb on the sketch you named Cover.

Press E to Extrude. Select the offset area (You may have to zoom-in to do this). Type in -2 for the distance and make sure the Operation is set to Join. It should look similar to this.

Press OK. You have made the cover’s lip.

We need to make a small clearance between the Cover and the Body. Press Q for the Press and Pull command. Select one of the sides of the lip. Change Offset Type from Automatic to New Offset. Select the remaining 3 lip sides by clicking on them. Set the Distance to -.1 and press OK.

Adding Material to Support the Indentations on the Cover’s Lip

First we will add some support material to the back of where the indentations will be. Select one of the inner short sides of the lip. Click on the Create Sketch icon. Fusion 360 changes to a 2-d view.

From the SKETCH-dropdown-menu choose Rectangle and then Center Rectangle. Move the mouse along the top edge of the face until a triangle appears. The triangle indicates the center of the edge. Move the mouse down and then click to set the center of the rectangle. Now drag the mouse to give the rectangle a height and width. Make the height 2 mm and width 10 mm. Press return. The rectangle is shown below.

From the SKETCH PALETTE, click on the Colinear icon. Select the top edge of the 2 by 10 rectangle, and then the top edge of the lip’s side. Fusion 360 moves the rectangle so its top edge is colinear to the top edge of the lip’s side (when the cover is right-side up).

Click on the STOP SKETCH icon. Press E to extrude and select the rectangle. Set the distance to 1 mm as shown below.

Now we chamfer the sides of the extrusion. Press S to bring up the Model Toolbox. Type in ch and choose Chamfer. Choose the edges and set the Distance to 1 mm as shown below.

Repeat the above to add material for the opposite indentation

Creating the Indentations on the Cover’s Lip

Select one of the outter short sides of the lip that corresponds to a nub. Click on the Create Sketch icon. Fusion 360 changes to a 2-d view.

From the SKETCH-dropdown-menu choose Rectangle and then Center Rectangle. Move the mouse along the top edge of the face until a triangle appears. The triangle indicates the center of the edge. Move the mouse down and then click to set the center of the rectangle. Now drag the mouse to give the rectangle a height and width. Make the height 1 mm and width 11 mm. Press return. The rectangle is shown below.

From the SKETCH PALETTE, click on the Colinear icon. Select the top edge of the 1 by 11 rectangle, and then the top edge of the lip’s side. Fusion 360 moves the rectangle so its top edge is colinear to the top edge of the lip’s side (when the cover is right-side up).

Click on the STOP SKETCH icon. Press E to extrude and select the rectangle. Set the distance to -1 as shown below.

Press OK. Now we will add a Chamfer. Press S to bring up the Model Toolbox. Type in ch and choose Chamfer. Select the bottom edge of the indentation and then the bottom edge of the lip. Type in 1 mm for the Distance and press OK. The chamfered indentation looks like this.

Repeat the procedure above to create an indentation on the opposite lip.

Acknowledgements

Many thanks to Nick at educ8s.tv . Nick made this video https://www.youtube.com/watch?v=YVNH0lBTdAI on using Fusion 360 to design a case. Nick’s enthusiasm for Fusion 360 inspired me to download and start learning it.

I watched two videos by Noe Ruiz of Adafruit to learn about nubs and indentations. The video Layer by Layer — Using Pattern on Path contains the details of making nubs. Noe’s second video, Layer by Layer MiniSpyCamera Part 2 shows how to do indentations in a cover.

I thank Autodesk for providing Fusion 360 free to hobbyists.