Making a hex grid in Fusion 360
Kimmy
Overview of the typical parametric design process
Fusion 360 doesn’t store polygons. Instead, bodies are stored as a mathematically exact representation of their form, which may include faces, spheres, curved surfaces, etc.
We modify these forms by adding features that add, subtract, or modify their shape.
UI overview
Timeline: shows the features you’ve added to your design
Properties of what you selected
Viewing cube!�(Mnemonic for the axes colors: RGB = XYZ)
Contents of your design (bodies, sketches)
Layout options (grid, etc)
UI overview
✴️ The most important (and often overlooked) part of the UI is the Timeline, right here.
Key idea: the features on your timeline are what define every aspect of your design.
Features, not polygons
Your timeline is a sequence of features (operations/steps).
In Fusion 360, we don’t edit model geometry directly – instead, we add features to the timeline, and each feature changes the body’s form in some way.
Example: this volcano has five features:
You can scrub through the timeline and add/remove features as you wish. The timeline isn’t related to undo history – you’re encouraged to add, edit, and even reorder features you’ve defined.
It’s good to keep clean timeline hygiene in mind as our designs unfold.
Parametric design in a nutshell
Designs in Fusion 360 are parametric, meaning that every feature is mutable and nondestructive.
Your timeline is a recipe. Later features build upon earlier ones, so edits to early features propagate through to the final result. This way, we can change our design without having to redo tedious modeling work.
Example: As I edit this first Extrude feature, watch how the later features get “replayed” on top of the modified design automatically.
👆🏻Double-click a feature on the timeline to edit it.
It starts with a sketch
Most designs in Fusion 360 start from a 2D sketch on some plane.
Select Create Sketch on the toolbar and select the XY ground plane.
Sketches are collections of 2D points, lines, and curves, paired with the Constraints that define them.
A closed collection of curves on a sketch makes a Profile that can later be extruded.
Sketching a shape
After we create a sketch, the camera rotates to view its plane directly overhead.
Now, select Create -> Polygon -> Inscribed Polygon
Click once on the origin point, then click anywhere else to draw the shape.
While drawing, you can also enter values and press “Tab” or “Enter” to finish. This will add additional Dimension constraints.
Sketching a shape - Constraints
The final shape becomes a Profile, a closed collection of curves with a light blue background
Underconstrained profiles show up with a blue border. Because they are underconstrained, we can drag these shapes around with the mouse. This may change their scaling, rotation, or even position, depending on the constraints in our sketch.
In this example, the only constraint specifies that the middle of the shape should lie on the origin. (See the pentagon icon near the center) We can’t move it around, but we can drag parts of the sketch to scale or rotate.
(If we clicked on the constraint and deleted it, we would then be able to move the shape around with the mouse.)
Sketching a shape - Constraints
Fully constrain your first shape by
Once a profile becomes fully constrained, its outline turns black and it can’t be dragged with the mouse anymore.
👆🏻 It’s generally a good idea to fully constrain your sketches.
Sketching a shape - Constraints
Constraints show up as little icons. They are first-class objects – you can select them and hit Backspace to get rid of them if your model is overconstrained. You can also double-click on Dimension or Angle constraints to edit them.
This hex has three constraints:
Sketching a shape - Offset
Add a 0.1cm offset around your hex.
Doing this creates a second profile around the first.
Both profiles remain fully-constrained.
Make sure that this becomes an offset rather than an inset! Negate the value if necessary.
Sketching a shape - Construction lines
We need to add two extra construction lines that will help us tile our hexes later.
Add a line going from the center of the shape to the midpoint of the outer side. You’ll need two of them.
Be sure to select the outer edge, not the inner edge.
Example: while drawing the first line, I hovered my mouse over the midpoint until I saw a blue triangle, which meant Fusion 360 would add a midpoint constraint automatically.
For the second line, I added the midpoint constraint after-the-fact, just to demonstrate.
Sketching a shape - Construction lines
Construction lines can help align geometry or apply further edits down the road. Construction lines are dashed, regular lines are solid.
What’s the difference? Closed regions that involve construction lines don’t become profiles, so they aren’t selectable as an area.
In my example, I can select the “pie slice” area separately, but this isn’t selectable after marking them as construction lines.
👆🏻Construction lines help convey the “engineering intent” of your design. You don’t need to mark them, it’s just a convention.
Sketching a shape - Construction lines
While we’re here, Inspect one of these lines and write down its length for later. This is half of the length we will need to offset each hex when we make the grid.
This one is 2.698cm.
Sketching a shape
We’re done here. Finish your sketch.
Your sketch is listed under the browser on the left hand side:
The red padlock means your sketch is fully constrained. If you instead see , you usually have more work to do, but that’s less important for simple designs.
From sketches to bodies
Add an Extrude feature. Click Extrude, then click the profile of your sketch. Type 0.5 and press Enter.
Your Extrude feature also shows up on the timeline:
If you need to change its parameters later, you can double-click it on the timeline to edit.
Because the default is “New Body” mode (see settings on the right), this extrude also creates a new Body in the browser.
From sketches to bodies
Unhide your Sketch, and add a second Extrude feature. Select the outer ridge and this time extrude to 0.7 cm.
This second Extrude also shows up on the timeline:
This time, the “Operation” is “Join,” so this feature gets joined to our first Body instead of showing up separately in the browser.
Patterns
Let’s fill our grid with hexes. Begin to add a Rectangular Pattern feature.
For “Objects,” drag-select your hex body, or click it on the browser.
For “Axes”, select the two construction lines you added earlier. (You may have to zoom in to select them.) These specify the 60° directions to tile along, rather than just the X or Y axes.
You can then begin to drag out your shape.
Don’t hit Enter yet.
Patterns
Let’s turn these clones into nice uniform grids.
First, set “Distribution” to “Spacing.”
We want to offset successive hexes in each shape by 2×2.698cm, the length of the construction line we made earlier. Enter “2.698*2” for both directions. (Math is supported in all text fields.)
Don’t hit Enter yet.
Patterns
Want more hexes? No problem.
For “Direction,” choose “Symmetric” for both axes, then bump up “Quantity.”
You can then turn on “Suppression” and uncheck hexes until you get a nice pleasing shape.
Hit enter when you’re done.
Patterns
Adding so many hexes filled the browser with many spurious Bodies! We need to combine them for export.
Shift-select them in the browser and add a � Boolean Combine feature. Once you hit Enter, only one body should be left.
Fusion 360 is awesome at booleans. You generally don’t need to worry about overlapping or nonmanifold geometry when using boolean operators on bodies (except in pathological cases).
Note: if this fails, double-check that your Rectangular Pattern feature’s “Distance” matches the length of your construction line. (See slide 15)
Preparing for export
In Fusion 360, all geometry is manifold and watertight by default because the boundary representation is mathematically accurate.
You’ll find 3D Print Export under “Utilities.”
Now is a good time to preview the resulting mesh and make sure it slices correctly.
Where to go from here?
CAD is a great jumping-off point to develop more skills. Learn by doing!