We all know and love OpenSCAD for its sweet sweet parametrical goodness. However, it’s possible to get some of that same goodness out of Fusion 360. To do this we will be making a mathematical model of our object and then we’ll change variables to get different geometry. It’s simpler than it sounds.
Even if you don’t use Fusion 360 it’s good to have an idea of how different design tools work. This is web-based 3D Modeling software produced by Autodesk. One of the nice features is that it lets me share my models with others. I’ll do that in just a minute as I walk you through modeling a simple object. Another way to describe what we’re going to learn is: How to think when modeling in Fusion 360.
Meet the parameters box. The parameters box contains every single dimension (variable) defined inside the model. You can also add your own. This is what we’ll be doing to make the parametric model.
For this tutorial we will be making a box to store small tools in. I recommend following along with the steps in the Fusion360 model. There’s a time line with playback controls at the bottom of the Fusion360 window. You can move the slider back and forth to see different stages. You can also right click on any of the steps and select, “Edit Sketch,” or, “Edit Feature,” to see particular things.
Before I even began making the box, I sat and thought about how I would put together the model. Since it’s parametric I knew I wanted as few variables as possible. I’d rather have the computer do the work for me. So I came up with five things that would define my box.
- Length – The length of the inside of the box. Since my box is for holding things I don’t care how big the outside is. I’d rather have the software calculate that.
- Width – The width of the inside of the box.
- Height – The height of the inside of the box.
- Thickness – How thick the walls and the lid are. I also derive the thickness of the ribs on top from this number.
- Fit – This is the fit/clearance between the lid and box. 0.25mm is pretty easy to hit for a well tuned printer.
Next came the sketch. When using any modern CAD software it’s important to keep in mind that what you are doing isn’t really drawing as much as it’s building a mathematical model of your object. I tend to think of the process as graphical programming. One mistake I see a lot of newbies make is to completely ignore the dimension tool (shortcut: D) and the constraints panel. The constraints tell the software that, mathematically, Line A is always parallel to Line B, or Circle A is always tangent to Line B. Grasping this lets you create models that will expand and adjust with changed dimensions and design considerations. It also dramatically speeds up your drafting time.
A few tips on the sketch:
- Fusion has some great hotkeys. Some of the ones I use are Q – Cut/Extrude (push/pull) the sketch, D – dimension, C – circle, L – line, and P – Project.
- Double check your constraints. Fusion is conservative about which constraints it places for you. Make sure the obvious ones are there.
- The parameters are case-sensitive. “Thickness,” is not the same as, “thickness.”
- I could sketch the box, and then using relations to the box, sketch the lid. However, if the shapes in the sketch aren’t touching they will be extruded as separate bodies.
Once the profile of the part was finished I selected the lid profile and the box profile and extruded the box. Again, since I want a parametric part at the end, rather than entering numbers during this step I enter in the variables I had set previously.
Right now the box is a lid and an extrusion without ends. I need to cap the ends of the box. To do this, I will use a plane and the mirror operation to copy the ends to both sides. If that sentence is off, another way to think of this is pseudo code.
Once it starts to click that you are not drawing the shape or modeling it in a traditional sense, Fusion starts to make a lot more sense. You are programming in a visual way. A side note, the mirror and pattern commands in Fusion are really cool, but complicated. I’d recommend watching a YouTube video if this function is giving you quirky results (Such as filling in all the empty space in your box).
Next I added some decorative features to the lid. This was similar to the previous steps: make a sketch that is dimensioned with the variables, then extrude or cut using the sketch. I used the slot tool to add ridges to the top for grip. After I added the ridges I drew a rectangle that cuts away some of the ridges so I can have an area to write what’s in the box.
Now it’s time to test the file. We’ll go back and open the parameters window and change one of the dimensions. Oh no! An error. Like any code, it didn’t compile the first time. In this case, when I drew the initial slot I didn’t have the midpoint of the slot constrained to the middle of the lid. I drew a line from one end of the box to the other, making sure to constrain each of its ends to the middle of the lid, and then used the coincident constraint to attach the middle of the slot to that line. Creating a mathematical relationship.
After fixing the sketch, I tried again. It works! When I change any of the values I get a new model of the box. As you can see in the opening image of this post! I used the make command to generate STLs for my printer. Then, admittedly, went a little overboard on the tiny boxes.