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Making Boxes in Fusion 360 for Laser Cutting

When making a box with a laser cutter, its entirely possible to make your design as a single flat drawing through careful planning and measurement – but who wants to do that!? This is a guide to making a box quickly and easily using Fusion 360. In this guide, we will cover the basics of box building, walk through how to make a simple scalable box, how to export in a usable format for a laser cutter, and share some helpful links to box making web apps.

Finished-laser-cut-box

Joint types

There are many different types of joints that can be used when making a box. We are somewhat limited to the type of joints we can make with a laser cutter since we can only cut straight down through the material. Let's start with the types of joints you can make with a single sheet of material:

Butt Joint - This type of joint offers very little security and is just two pieces butted together.

Example-of-a-butt-joint

Finger Joint - This is what you see on most laser cut boxes. It offers slightly more mechanical strength than a butt joint, but if you need it to stay together you will need to glue it. A well-focused laser cutter will make a snug fit with a finger joint.

finger-joint-example

Mortise and Tenon - With the mortise and Tenon we start to get into joints that offer real mechanical strength without relying on glue. One of the pieces sits inside a recess in the other piece and effectively prevents motion in one plane. A variation of a mortise and tenon can be a hook, which offers even more strength since it prevents the pieces from easily pulling apart.

Mortise-and-tenon-example

Snaps - There are many different types of snapping connections, we all know them as that broken part that used to hold the battery cover on your remote control. Snaps can be hidden or with the tabs exposed and can be a great way to hold a box together. Combine it with Mortise and Tenon for extra strength!

Snap-joint-example

Complex Joints - There are many more types of joints out there that are achievable with a single flat piece of material. If you want to make more complex joints you can engrave grooves in your material to make sliding dado joints, rabbet joints, and lap joints. Stack two or three sheets to make dovetail joints!

Hook-joint-example

Building with Parameters

For this project, we are going to be using parameters to build the box. Whenever possible it’s a good idea to make your boxes this way, because it allows you to scale your box or change the thickness of the material without remodelling. You do need to be pretty intentional about the way you design it for it to work properly though. A parameter is a user set variable, that we can use for dimensions in our design. You can even include some simple math in your dimensions fields that involve parameters. We will be making a cube, so we will make a single parameter for Width, and we won't worry about Depth or Height since it will be the same. This does limit the design to forever be a cube though. We will also create a Thickness Parameter of 3mm.

assigning-parameters-in-fusion-360

If you design your box carefully using parameters and constraints for your dimensions, then you end up with a scalable box that you could make out of different materials later on.

Draw the Box

Let's break it down into steps, Width = 60mm and Thickness = 3mm. I will use parameters for all my measurements so the drawing will be scalable:

  • Construct an offset plane from the Z-Plane. Offset it .5*Width. This is where those user parameters come in handy. Create a sketch on the plane and draw a centre point rectangle that’s Width X Width.

user-parameters-in-action-fusion-360

  • Draw two fingers using the line tool starting from the edge. Set the measurements to be Thickness and Width/6 respectively. We now want to add construction lines from the fingers to the edge of the square and constrain them to be equal. Give one a dimension of Width/6. It might be worthwhile to check to see that your drawing scales at this step by changing the values in your user parameters. It's good to catch these problems early.
  • Now we will select the fingers and construction lines and do a 4X circular pattern around the Origin, This will copy the fingers to each edge. We can now extrude the bottom plate by “Thickness”.

bottom-plane-sketch-box-making-fusion-360

  • We will repeat these steps with a vertical plane, but we only need to draw our fingers on one vertical side. Extrude the sketch.

Side-panel-sketch-fusion-360-box-making

  • Use the Combine tool to Cut fingers into the bottom of your vertical panel by using the bottom panel as a tool, select “Keep Tools”.
  • Select the vertical body and do a Circular Patter X4 to copy it around the box. Repeat the Cut command to cut fingers in the overlapping vertical edge of each piece.

Fusion-360-box-objects

You're done! Convert all the bodies to Components for clarity and you’ve got a scalable box on your hands!

fusion-360-box-components

Prepare the Model for Laser Cutting

To get a usable file for laser cutting, we need to lay all the panels flat on the same plane. Let's use the Z-plane. Using the Align tool under Modify, select the outside of a vertical panel and then the bottom of the bottom panel. This will move the side panel to be on the same plane as the bottom panel (and in the same spot). Move all the panels away from each other so they are no longer overlapping. Position them close together and in a position that makes sense for you laser material.

fusion-360-box-parts-laid-flat

Once all the components are positioned use the Project tool under Sketch, and select the top face of each panel. This will create a new sketch with the outline of each panel. Navigate to the newly created sketch in the Browser and right click on it to select “Save as DXF”. You can now open that DXF in a vector editing software like Inkscape and change the colour and size of the lines to red with .01mm stroke. Your file is ready to be sent to the laser cutter!

Laser-cutter-cutting-box

Finished-box-laser-cut

Going Further

Now that you’ve gotten your feet wet with a little laser cutter box building. Try out some more complex joints in your boxes! If you want a little inspiration, check out the design of the box that we created in this tutorial, or a Project Box for the Circuit Playground Express that uses mortise and tenon, hook, and clip joints for a very strong box with no fasteners!

There is a great web tool designed for making boxes called Boxes.py. It was a featured project over at Hackaday.io and is a great tool for making boxes up quickly! It also does hinges, lids, pulleys drawers and parametric kerfs.

To learn more about laser cutting, check out our online laser cutting tutorials and guides, and if additive manufacturing is more your thing, we have a whole library of 3D Printing Tutorials. Don’t forget that we offer a Laser Cutting Service, send us your .svg files and we’ll cut it and send it to you!

If you are looking for some more joint inspiration, Make has a great article on CNC joinery that applies to laser cutting

For some incredible joints, check out The Joinery on Twitter!

When making a box with a laser cutter, its entirely possible to make your design as a single flat drawing through careful pla...

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