Creating Radially Intersecting Features: Designing and Using Complex Lap Joints

Hi there! I'm a student at the University of Victoria (featured in this Instructable) in British Columbia, Canada.

When I started making ridgeline maps, I thought it might be neat to do one that focuses on just a single mountain peak instead of a whole region. Contrary to a traditional contour map or my earlier ridgeline designs, my idea for the mountain involved the ridgelines spreading out radially from the summit.

Now almost a year later, I was finally getting around to actually making the mountain ridgeline models (for which the method of getting/processing the data will hopefully be a topic of a future Instructable!) and realized how complicated it would be to try and get multiple pieces aligned radially! I certainly considered doing what I did for the layout of the globe model I made last year and just aligning pieces onto a central core or frame, but thought it might be kind of fun to explore more generally how to stack and slot things vertically/radially with no interference between pieces or wasted open space in the middle.

I searched for things like "slotted", "radial", "interlocking", "notched", "overlapping", "intersecting", etc., etc., etc. and I couldn't find any good examples for how to do this. If you have any sources that I missed or keywords that could be helpful, please let me know!

If you're just interested in the SVG files for the things shown in these images, you can find them in Step 10 :)

The primary purpose of this Instructable is to:

Illustrate the process used to set up and visualize the interlocking pieces,
Demonstrate how to expand to additional numbers and configurations of pieces, and
Show a few examples of how this process can be used to make cool things!

Supplies

Fusion 360: I originally tried to figure out laying all the pieces out in Inkscape and was wary of Fusion 360 because I:

Didn't really want to have to install/learn a new software, and
Have an almost decade-old laptop with not much space left on it and was worried that I'd overburden it!

It ended up working out great though (minus one hiccup when it started updating without warning and slowed my laptop to a crawl*) and it was nice to get some experience with a new, very capable software!

Material for cutting: My projects are mostly made out of wood, but pretty much anything should work!

Laser cutter[optional]: I'm fortunate that the makerspace where I'm a member has a laser cutter available for me to use, so that's how I put together my projects. The cuts for the interlocking slots themselves are pretty straightforward though, so as long as you don't have a really complicated profile or hundreds of pieces, cutting the slots by hand should definitely be possible!

*Quick tip: if you're experiencing this and don't know what's happening, the "Job Status" icon will tell you if Fusion 360 is updating. I had no idea until I did some digging!

Step 1: Goal: 16 Interlocking Pieces

This photo shows a top-down view (from one of my original Inkscape trials) of what the end goal of this process is with 16 features aligned radially. Note that each piece (except the top one) is shown with a gap between its two halves but is actually connected lower in the stack with what I'll call a "tab".

The left side of the photo shows how the pieces are arranged at angles to one another:

Group 1: 1 piece at 0 degrees
Group 2: 1 piece at 90 degree angle to #1
Group 3: 2 pieces at 45 degree angles to #1 and 2
Group 4: 4 pieces at 22.5 degree angles to #1, 2, and 3
Group 5: 8 pieces at 11.25 degree angles to #1, 2, 3, and 4

If you notice a pattern between the number of pieces and the group that they're in, that will come up later!

The right side of the photo just shows the pieces color-coded (darkest to lightest) by their group.

Step 2: Use the Right Angles to Minimize Cutting!

Big themes

Literal right angles are one of the keys to making this project work. Notice in the previous step that each piece of the array has one other piece that's perpendicular to it within its group (matched by color in this image). Aligning pieces perpendicularly reduces the size of the slot required to fit them together to a minimum. The farther you deviate from 90 degrees, the larger the slot has to be, so its best to layer things in such a way that the relative angle between two (vertically) adjacent pieces is maximized.

Because of that, it doesn't make sense to start with piece 1, put piece 2 on top of it, etc. Instead, we'd start with piece 1, jump to piece 9 (90 degrees to piece 1), then piece 5 or 13 (45 degree angles to pieces 1 and 9), etc.

Step 3: Overall Dimensions and Slot Size

The plywood that I'm using for this project is 2.9mm thick, so I designed for that as it's important for the width of the slots!

I had a nice strip of 40mm tall plywood leftover from another project, so I figured I'd use that if I could! For 16 interlocking pieces, that means the thickness of the tab connecting the halves of each piece will be:

40mm tall / 16 pieces = 2.5mm tab

The width of each piece doesn't matter too much (as long as it's wider than the widest slot cut! See below for calculating), so I just made it an even 35mm wide.

So each piece with no slots cut in it will be 35mm wide x 40mm tall x 2.9mm thick with a 2.5mm middle connecting tab. The first photo shows a "full" piece with no slots cut in it.

Calculating slot size

The required slot size is based on the relative angle between two pieces and the thickness of the material being used.

As shown in the second image, we need to figure out the width of the parallelogram that represents the intersection of the two pieces. It is a regular parallelogram, so all 4 sides have the same length.

Therefore, using some trigonometry, we come up with this equation for the width of the slot:

w = t / sin(α) + t / tan(α)

w = t * (csc(α) + cot(α))

where:

w is the width of the slot
t is the thickness of the material
α is the angle between the two pieces

So for my 2.9mm thick material, the widths of the slots that I'll need eventually are:

90 degrees = 2.9mm
45 degrees = 7.0mm
22.5 degrees = 14.58mm
11.25 degrees = 29.44mm

Did we really need to do that calculation?

Not at all! Using Fusion 360, we can easily just draw the rectangles that we need by referencing existing geometries, so no need to do any math. I just think it's kind of nice to figure out the math behind what's happening when we do that!

Step 4: Starting Small

EDIT/UPDATE!

I've played around with Fusion 360 more since publishing and would recommend using the extrusion tool rather than push pull in later steps as it allows you to more easily join new features to existing components rather than doing that as a separate process.

The initial sketch

Rather than starting with a full size (35mm x 40mm x 2.9mm) piece of the array, I found it was much easier to start with just a single section equal to the height of the tab that will connect the two halves of the pieces.

In my case, that tab will be 2.5mm tall, so my starting piece will be 35mm wide x 2.5mm tall x 2.9mm thick

I sketched this on the top plane as a 35mm x 2.9mm center rectangle with its center at the origin. The rectangle is centered on the origin so that rotating it about the Z axis in future steps will be simple.

The initial solid

The sketch is then Extruded to a distance of 2.5mm using a "One Side" extrusion. It's extruded to just one side because pieces in future steps will be mirrored across the top plane.

Step 5: Planning Ahead

To avoid having to create new rectangles using the equations shown in Step 3, we'll instead create a set of sketch geometries that can be used as references for future 3-dimensional features.

To do this, I created a new sketch which:

Copied the geometry of my initial sketch (using the "Project" sketch tool in the Create menu), and
Created a rotated array of additional rectangles using the Circular Pattern tool
Use "Angle" for Angular Spacing
Like many other programs, Fusion 360 includes the original feature in it's count when making arrays, so the Quantity should be 16.
The "Total Angle" is a bit tricky. You'd think it would be 180 degrees, but if we had the initial sketch rotated 180 degrees, it would just end up laying directly on top of itself. So instead, the "Total Angle" should be 180-11.25, or 168.75 degrees.

It definitely looks a little busy, but once you know what to look for later it's not too bad!

One handy tool that I learned about when doing this is "chain selecting" geometries. When projecting geometries, it's convenient to select all of them at once rather than selecting individual line segments. If you double click on a sketch, it will automatically select all connected lines instead of just one at a time! It doesn't seem to work for doing Circular Patterns though, so I think you have to select each line individually for those (if someone who knows Fusion 360 better can confirm or deny this, please let me know as I am still new to the program!).

Step 6: Building Up

Each additional layer that is added to the model consists of a copy of all existing features that are then flipped and rotated to slot into the gaps between pieces of the previous layer. This step just describes the overall process. Step 7 goes through an example for the first 3 groups (0 degrees - 1 feature, 90 degrees - 1 feature, and 45 degrees - 2 features) with attached images.

Overall Process

Preparing existing features

For each additional layer, a new sketch is created on the top (or bottom) faces of the existing geometry.

This new sketch:

Represents the area that is not cut out of the existing feature to accommodate the intersecting angle of the next group.
This step uses the sketches created in Step 5 as reference geometry
Is "Press Pull"-ed to a distance equal to the height of the existing features.

Interlocking features

With the features created with the new "Press Pull" sections on them, they can be duplicated, mirrored, rotated, and translated.

Step 7: Building Up Example - Groups 1&2

If the previous step sounded a little confusing, hopefully this example will help!

The first image shows the initial extruded solid that was created in Step 4.

Using the process shown in Step 6, we'll do the following:

Create a new sketch on the top face of the feature (right-click > Create Sketch)
The next group is the 90 degree group, so we'll find the rectangle in the radial array of sketches that is at 90 degrees to the existing feature (you may need to turn on the visibility of that sketch)
Click on the two long lines of the 90 degree rectangle (click + Shift +click) as shown in the second image.
Click Create > Project / Include > Project
Be sure to select Construction as the Linetype in the Sketch Palette as shown in the third image
Hide the radial array sketch
Draw two rectangles on the face of the existing feature (deselect the Construction Linetype!). It should be easy to snap them to the intersection between the projected geometry and the edges of the existing feature face (shown in fourth image)
On the Modify tab, select Press/Pull
Select the two rectangles as the profiles
Distance should be equal to 2.5mm
All other settings should be the default (as shown in the fifth image)
Right-click on the body in the Browser panel on the left and click "Create Components from Bodies".
This will turn the feature into a component. A component is needed because, as far as I'm aware, Fusion 360 will not let you copy and paste Bodies without them being linked. We'll need to make changes later that need to affect only individual pieces, so Components are necessary for that.
Right-click on the newly created component in the Browser panel and click "Copy"
Click somewhere in the main window (not on the component) or hit the Esc key to deselect the component
Right-click anywhere in the main window and click "Paste New" to create a new component that's not linked to the original.
In the Move/Copy menu that pops up immediately after you paste (shown in last image):
Click on the icon next to Set Pivot, select the Origin (O) from the Browser panel, then click the check mark icon that is now next to Set Pivot.
Change the Z Angle to 90
Change the X Angle or Y Angle to 180
Change the Z Distance to -5mm (2.5mm tab thickness x 2)
The preview should show up to show you what it will look like! If that doesn't look right, you may need to change a few parameters, make sure you've selected the proper origin, etc.

At this point, it's probably a good idea to rename your components so that you can keep them straight! I just renamed mine Group 1 and Group 2.

Step 8: Building Up Example - Group 3

As indicated in Step 1, Group 3 is made up of two components that are at 45 degree angles to Group 1 and Group 2.

It turns out that Group 3 is just a copy of the combination of Groups 1 and 2 (with the Press Pull sections created).

Follow the same process shown in Step 7, but create the rectangles using reference geometry from the 45 degree radial sketches instead of the 90 as shown in the first image. It doesn't matter which component you select to draw the sketch on, but you also need to select the outside edges of the face of the other one to Project sketch geometry as well, otherwise the rectangles won't snap to those corners.

The Press Pull distance for this one is now 5mm, because that's the total height of Groups 1 and 2 combined. If by chance the Press Pull doesn't join each new section to its original component (as it did with mine a couple of times and I'm not entirely sure why...) you can use the Combine tool to merge your target body (original component) and tool bodies (the newly Push Pull-ed bodies).

The attached images show Groups 1 and 2 with their extended sections (image 2) and Group 3 created, rotated, and translated (image 3).

Step 9: The Final Group!

Repeat the process shown in Steps 7 and 8 until you've filled in all angles.

Group 4 should be rotated 22.5 degrees and translated 20mm and Group 5 should be rotated 11.25 degrees and translated 40mm.

The final result should look something like what's shown in the image.

One fun thing you can do in Fusion 360 is click "Display Component Colors" in the Inspect tab dropdown, and it will color each component separately as shown in the second image.

Step 10: What Next?

Using this method, you can make all sorts of neat things! Using the Shaper Utilities addon for Fusion 360, it's relatively easy to export SVG files that can then be cut on a laser cutter (or by hand if you're feeling ambitious!). My process is to export to Inkscape for final setup (checking dimensions, assigning line colors, etc.), then from Inkscape to Lightburn (a laser cutter software) for arranging pieces based on the wood that I have available.

As shown in the intro image, I made a little cylinder, ball, and ridgeline model of Mount Fuji, which will hopefully be turned into its own Instructable at some point in the near future :) The cut files for these models are attached here in SVG format.

Mt. Fuji model file

The Mt. Fuji model is designed for use with 1.7mm thick material (this was the measured thickness of my 1/16" plywood) but can be easily adjusted using instructions included in the file.

Example svg file

The ball and cylinder in the examples file are designed for 2.9mm thick material but can also be easily adjusted. The cut pattern included in the example file can be used for making any shape you'd like! Just subtract it from the shape you're working with and be sure to extend the bottom and top of the cuts through the bottom and top of the material you're working with if needed.

Note that this file only includes 8 shapes for each model but the whole model requires 16 pieces! That's because each half of the model is identical so only 8 unique pieces are required.

Lots of different things can be made using the same basic pattern! Once you have the slot cut shapes available, slotting together all different shapes is possible. Scaling both horizontally and vertically is simple to accommodate different thicknesses and heights of wood.

I'd like to explore these types of designs more. For example, splitting angles in half creates 1, 2, 4, 8, then 16 features, so it's clearly a base-2 system. What happens if you trisect angles instead? Or combine different methods - a clock face, for example, is split in half twice, then into thirds. How easy would it be to change the method to make that possible?

As always, please share what you come up with if you try this out and let me know if you have any questions or comments! Thanks!