Registration

1. Go to Educational Use for Fusion 360 from the Free Trial page

2. Sign in to your Autodesk account and follow the instructions onscreen to obtain your license/download the installer.

3. Install as you would any other software.

4. Once the software loads, sign in using the button in the upper right corner.

Fusion360 is a cloud-based Computer Assisted Design software from Autodesk. At TJUAV, we utilise Fusion360 to collaborate on designs and create 3D models of our system for manufacturing, modeling, and simulation. This section of the documentation goes over the first steps for installing and beginning work in Fusion360. This is not a guide of 100% of Fusion, but if you hover over a tool you're unsure about, a description will appear. In addition, there are many tutorials online, and the members of TJUAV are always happy to explain something you don't understand. All you have to do is ask.

Create Menu

Last updated 3/24/2021

Modify Menu

Combine

Select the Target Body (body which has the action performed on it), then select all the tool bodies.

Join - Joins bodies into one large body as long as they are touching.

Cut - Cuts tool bodies out of the target body (especially useful when combined with Offset Face because you can make perfectly contoured holes in objects, similar to a mold).

Intersect - Keeps only the intersection of the target body and the tool bodies (useful for making wing ribs because you can first Sweep the wing shape, then Rectangle Pattern a series of rectangular prisms down its length, and finally Intersect the sweep with the prisms to get the ribs).

"Keep tools" allows your tool bodies to remain, otherwise they get merged or deleted in the Combine tool.

Split Body

Using a plane, face, or profile (mostly planes) it splits a body into two pieces along that plane. This is very useful for cutting large objects into smaller pieces, such as cutting an aileron from the wing.

Construct Menu

Making planes and axes is a must have skill for any person doing CAD. Although this menu's tools are self-explanatory, people don't know when or how to use its tools in creative ways. This, however, cannot be taught through this documentation and only is learnt through practice. See Smart CAD Tutorial (making a file) for a slight lesson on this.

Sketches

Sketches, located under the Create menu, are constrained drawings on a 2D plane or surface, and the first step to any CAD model. To start a sketch, you click the Create Sketch button. Afterward, select a FLAT plane (could be your origin planes, planes you created, or a face of a body). Once within a sketch, you have access to sketching tools, which differ from normal tools.

Remember to use Construction Lines to define objects without splitting faces in your sketches. To make a line a Construction Line (invisible, dotted line) click the line and then click the X key.

Constraints

When making your sketches, make sure your lines are all black (this means that they are fully constrained). If the lines are blue that means the lines have some permissible range of motion, which you can see by clicking and dragging the line (note, sometimes the line or curve will not move because it is constrained in such a way that it has two unique positions; in other words, maybe it doesn't slide but it can be mirrored). If the line isn't fully constrained it may move in an unpredictable way when dimensions are changed. There are many ways to prevent this, and often times you'll need more than just one of the following tools:

You should NOT rely on the Horizontal/Vertical constraint because this defines itself based upon the arbitrary orientation of the sketch. In other words, if you constrain a rectangle's sides as horizontal and vertical, you will never be able to rotate it in the future. If you would define the right angles instead, you could rotate the rectangle based upon an angular dimension you define.

Dimensions

The most crucial part of sketches is dimensions. Dimensions are used to constrain sketch objects based on length, angle, etc. To open the dimension tool, the easiest thing to do is click the D key. Then, click whatever you want to dimension.

• For the length of the line, click the line.

• For the angle between lines, click the first line and then the second line.

• For the distance between points, click the first point and then click the second point.

Instead of just defining the length of the line (or distance between two points), you can define the distance in a single or multiple dimensions. To do this, move your mouse to the side instead of directly away from the line, as pictured.

Remember to ensure you define the correct dimension in your drawing, for example, radius vs diameter.

CAD designs change frequently. Just as code uses variables to allow a single value to change, Fusion360 uses parameters. If a dimension changes, you can modify the value of the variable instead of altering sketches or timeline features. When setting a dimension, always set it to a parameterized value. To access parameters, click on the Modify menu, and then Change Parameters.

Parameters must match the dimensions of what they describe (you can't change this later!). Angular measurement must be made in degrees or radians, lengths in some form of meters, etc. Parameters can also be based on other parameters, and functions like add, multiply, square root, etc. can be used directly in the parameter value.

Once you have Fusion360 downloaded and installed, talk to one of the CAD team admins and have them add you to the team. Once you have been added (you'll need to accept the invite through email!), go to the upper left-hand corner of Fusion and click the dropdown next to your name. This will allow you to change between your individual and shared folders, and the TJ UAV files.

Joints

In the Joint tool, order matters when you select two components. An example of this is the Pin-Slot joint which requires the Pin to be selected first and the Slot to be selected second.

When selecting your component, you can use snaps. If you highlight the edge of a hole you will see a snap in the center, but when you try to hover over it, it can sometimes disappear. If you hold CTRL down, Fusion will allow you to select any of the snaps on your highlighted surface by ignoring any other surfaces you may hover over.

Joint Types

Rigid - Just like super glue, you ain't moving that any time soon.

Revolute - Synonymous with "rotation." https://youtu.be/PGNiXGX2nLU?t=61

Slider - It slides.

Cylindrical - Like a syringe, you can push, pull, and spin! (mixture of revolute + slider)

Pin-Slot - Like that type of chain lock that you put the bolt in the hole and slide it to the right.

Planar - Like a penguin on ice, you can slide anywhere on the plane, but you sure can't fly up or faze through it.

Ball - Lots of motion.

Joint Constraints/Limits

You first have to select the type of movement you want to constrain: Slide, Rotate, etc. Then you will select whichever constraints you want and define them. "Rest" just means whatever the default position is. The animation shows you the range of freedom.

Interactions

Multiple Joints on a complex object can work together to simulate the movement of a whole system! For example, a piston turning an axle can be simulated:

1. Stationary surface has Revolute joint with piston housing.

2. Piston housing has Slider joint with piston.

3. Piston has Cylindrical joint with wheel on the outer radius.

4. Wheel has Rigid joint with axle. (Rigid joints can move and turn in space if the component they are attached to is moving/turning, they aren't permanently jointed to a certain orientation or point in space)

5. Axle has Revolute joint with stationary surface.

Assemblies

To make an assembly, drag in files from the file menu on the left and they should appear in your file. Join these together to assemble your object. Whenever you change an individual object, it will update in your assembly because the change makes its way up the file tree.

Timeline Organization

At the bottom of the design workspace, for most files, you should see a timeline of all of the things added to the file. This is not the same thing as an edit history, instead, think of it more like the series of instructions the software is using to generate your objects. If your file does not have a timeline, for instance, if it's an imported file, you can create one by right-clicking the parent component in the tree and toggling timeline capture.

Redundant/Excessive Sketches

Projections/Arbitrary Definitions

Line Colors/Overlapping Lines

Design Resiliency

Component Nesting

Commit Messaging

Shortcuts

In Solid workspace:

• S - shortcut menu (search for tools)

• I - measure

• J - joint

• F - fillet

• M - move

• E - extrude

In Sketches:

• S - shortcut menu

• L - line

• R - rectangle

• C - circle

• P - project

• D - dimension

• O - offset

• T - trim

• M - move

• I - measure

Naming Convention

Timeline

Another basic concept in Fusion is a series of events. Many different operations may need to be performed to create complex shapes, and Fusion keeps track of this in the Timeline. Different icons represent different operations, like New Sketch, Extrude, and Revolve.

Anything before the slider is what is computed by Fusion (visibility depends on your own visibility settings in the browser and nothing after the slider will be computed until you move the slider past it). As a result, when you edit something earlier in the timeline, always move the slider back first before making changes and then slowly move it back to the present to make sure that any errors along the way are relatively easy to fix. Otherwise, errors propagate more errors, so a simple fix of one error could have prevented fifteen others that appeared, but once those fifteen appear, fixing the original error doesn't do anything because it's too late.

You can drag things around to change their compute order, but you are limited by dependencies between objects. For example, an extrude based on a sketch cannot be dragged before the sketch and vice versa.

Errors

There are many different errors associated with different tools, but their fixability depends on how well you made your CAD and how volatile the tool is. Sketches with projections, for example, are virtually unfixable unless started from the beginning. Sketches without projections solely may need you to redefine their plane. Other tools may throw a temporary error but if your open them up and click OK then they may resolve. Fillets and other tools under the Modify menu are often unfixable.

Components allow you to make , which are very important features in CAD.

Components allow you to organize all of your actions relating to a part together.

Activating Components

To activate a component, click the small dot to the right of the component you want. This will gray out any component or body that is not a subcomponent of your selection.

If something is grayed out, you cannot interact with it (AKA, Extrudes won't cut through grayed components). Keeping your CADs organized is very important, so always remember to use components wherever it makes sense to do so. A final benefit of components is that you can toggle visibility of objects more easily; for example, it is much simpler to turn on the sketches relating to a component than to sift through all your sketches in the main file to find out which ones relate to that one component.

Sketch tools are used to create specific features within the sketch environment. The key to correct usage of sketch tools is understanding each one's function. This page details more advanced tools and the benefits/drawbacks of using them.

Create Menu

Lines and Polygons

Specialized

Mirror

Pattern

Project/Include/Intersect

The P key, or a visit to the Create menu highlights a useful tool known as the Project tool. This tool creates a projection of any body, feature, component, etc. onto your sketch that allows you to use those lines as a reference. This is a very good tool for lazy CAD because it allows for thoughtless projecting without much understanding about properly defining things. As a result, when changing parameters, scaling objects, or doing changes backwards in the timeline, you often run into errors with your projections that cause irreparable chaos and eventually a full reCAD of that sketch and everything after it.

The Intersect tool has the same instabilities, but is used to detect the surface, line, or point with which a body, plane, or line intersects your sketch plane. Whatever you are projecting must intersect with your sketch plane.

Modify Menu

Fillet/Chamfer

Just like in the Solid workspace, the fillet and chamfer tools perform the same operations but within a sketch. Using them is unadvisable because although they save on computing power, editing them is a pain, they remove constraints that keep your lines black, and they perform function limited within the plane you are working in (the Solid workspace Fillet/Chamfer is much more useful because it works in 3d).

Trim/Break

Same downsides as the Fillet/Chamfer tools. The Trim tool (shortcut T) and Break tool help clean up your sketch and remove extra line endings and other unwanted things. The Trim tool is most useful when you make a line of arbitrary length in one direction (because you don't know its exact length yet) and then intersect that line with one coming at an angle that you have already defined. Trimming that extra length of the prior line is an easy way to save a few seconds that it would take you to use the Coincident constraint on both other lines' endpoints.

Offset

The most stable tool in the Modify menu is the Offset tool (shortcut O). This simple tool is probably the only too that it much more useful within the Sketch environment than in the Solid workspace. It is very simple to use.