Autodesk Fusion 360 is gaining traction with machine shops, students and hobbyists, and many of them are looking to up their game and become more productive with this great CAD tool. With this in mind, I want to share some tips that have helped my students when using the software.
Adding Custom Keyboard Shortcuts
Keyboard shortcuts are a great way to speed up workflow. I highly recommend you create a table with your favorite keyboard shortcuts and post it on your cubicle wall for easy referral. Most users select the same commands over and over, like line, circle, center rectangle, etc. Instead of having to move your mouse and search for the same tool, a shortcut key allows you to simply press one or two keys on your keyboard.
- Make a list of your most used commands.
- Locate a command in your list.
- Once you find your command, hover for a second and then hit the three vertical dots. Shown below.
Notice that the Center Diameter Circle command already has a shortcut key assigned, the letter “C.”
The menu allows you to Change Keyboard Shortcut. Select that option.
Shortcut keys can only be a single character—after all, they are supposed to be a shortcut—or a single character combined with holding down Shift, Control, Alt or Tab.
Once you have assigned the key, press OK.
Your shortcut key is now displayed next to the command.
Unfortunately, there is no way yet to print out all your shortcut keys. Autodesk plans to add that as a feature in a future release. The nice thing is that your shortcut keys are saved regardless of what device you use to access your seat of Fusion 360.As long as you sign in with the same account log in, your customizations are saved.
View Reset
This is a problem my students have all the time. They create a model, and then the views aren’t set up the way they want because they created the features on the incorrect plane. Another situation is when you download a model from a vendor site and import it, and the part is oriented in an odd way for the same reason.
In this case, I imported a vendor’s STP file of a connector into Fusion 360.The connector is lying on its side, so I want to re-orient it so it sits correctly.
I click on the viewcube and select the front view.
The connector reorients to show me the top view.
Right click on the viewcube and select Set current view as →Top.
You have now re-assigned this orientation as the top view.
Check this by setting the view to the Default or Home isometric.
I check my new Front view, and it still isn’t correct.
Use the arrows on the viewcube to rotate the view.
Now, my front view looks correct, but I need to save this orientation.
Right click on the viewcube and select Set current view as →Front.
Double check to see if the model views work the way you want by selecting a different view orientation.
Check your model against the viewcube to verify that it is oriented correctly.
Activating the Midpoint of a Line
Let’s say I want to place a circle at the midpoint of this line. How do I locate the midpoint? I start my circle command and hover my mouse over the line. When I see the triangle symbol indicating the midpoint, I left click to place the circle. It’s as easy as that.
Avoid Unwanted Sketch Constraints
It’s nice that Fusion 360 tries to help you by automatically adding sketch constraints, but sometimes the software is too helpful and adds constraints you don’t want or need. To avoid this, you have to be watchful. As you sketch, Fusion 360 will display a tooltip for the constraints being added. If you see a tooltip for a constraint you don’t want, press the Control key. That will prevent Fusion360 from adding that constraint.
Show and Modify Sketch Dimensions
To display the dimensions for a sketch, right click on the sketch in the browser. Then, left click on Show Dimension.
The sketch dimensions will appear.
To modify one of the dimensions, simply left click on the text and change the dimension value.
When you press Enter, the sketch and feature will automatically update. This also saves you time because you didn’t have to open up the sketch to make a quick change.
Once you are done editing, simply right click on the sketch again and select Hide Dimension.
Exporting Fusion3D Files to Different Formats
Right now, the Export Options for Fusion3D are a bit limited. Hopefully, they will expand in the future.
To export to a different file format, you can go to File→Export.
Your choices aren’t bad—IGES, SAT, SMT, or STEP. However, they aren’t great, especially if you want OBJ or DXF. If you want more options, click on the version number of the design in the data panel. Then select “Open Details on web”. Alternatively, go to File>Open Details on Web.
This will allow you to download other file types that are not installed locally by using cloud translators to translate your files to the requested file format for export. If you have a Team Fusion account, you can also upload the file to the cloud and export to DXF, DWG, OBJ, as well as other file formats.
Sharing Files on GrabCAD
I use GrabCAD as my go-to platform when I want to collaborate on a project or share a file. I simply upload to GrabCAD and then send an invite to my other team members. How cool is it that Fusion3D has a built-in menu selection that allows you to publish to GrabCAD? Just go to File→Share→Publish to GrabCAD.
A dialog will come up asking for your GrabCAD login. You can create a free account on GrabCAD’s website, if you don’t already have one.
If you have a free account, you can publish to the community. If you pay GrabCAD a subscription—I do because I love GrabCAD—you can publish to your Workbench, which is a private invitation-only cloud storage area where you can collaborate on projects.
You will see a short uploading animation.
Depending on the size of your file, there will be a short pause, and then the file will be available for viewing.
Clicking on the View Your Files link will open a browser and take you to the GrabCAD site, where you will have to log in again, but you will be taken directly to the project you just uploaded.
Using Selection Filters
When you are sketching or mating, sometimes you have problems selecting exactly the right entity. This is when Selection Filters can really reduce your frustration. Simply go to Select→Selection Filters and enable the entity types you want to use for your operation. By default, Select All is enabled. I find this annoying because it can interfere with what I want to do when everything I hover over highlights. By disabling Select All and only enabling the entities I am interested in, it makes it easier for me to move forward with what I need to do.
Dimensioning from an Arc or Circle Quadrant
Sometimes you want to dimension from the quadrant of an arc or circle. To do that in Fuson360, start the dimension command, hover over the arc or circle to be dimensioned, right click and select Pick Circle/Arc Tangent.
You can then select the quadrant points of the desired objects to place the dimension.
Making Components in an Assembly Selectable/Unselectable
When working in an assembly, there may be times when you want to add components with mates, but you don’t want to inadvertently select the wrong component to use for the mate. Highlight that component in the browser, right click and set it to Unselectable. This will keep it visible but allow you to ignore it for mating and sketching purposes.
To learn more about Fusion 360, read the recent engineering.com research report The Best CAD System for the Modern Engineer.
Autodesk has sponsored this post. They have had no editorial input to this post. All opinions are mine. —Elise Moss