Top 10 Productivity Tips in Fusion 360

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1 CP11251 Top 10 Productivity Tips in Fusion 360 Taylor Stein Autodesk Inc. Learning Objectives Learn how to speed up Fusion 360 workflows Learn how to make your selections even easier Learn important best practices and hard- to- find tricks Description Already a Fusion 360 software user, but want to learn some expert tips from the pros? Speed up your workflows and make sure you re utilizing all of the capabilities in Fusion 360 to make you even more productive. Even if you re new to Fusion 360, learn the tricks of the trade to get you off on the right foot. Your AU Experts Taylor Stein is a Mechanical Engineer by trade, and has been a Technology Evangelist at Autodesk for the past 2 years. Primarily focusing on Fusion 360, Taylor aims to inspire and enable the next generation of engineers, designers, and makers. Additionally, he works hands- on with startups in the San Francisco Bay Area that represent the future of making things, ensuring Fusion 360 and other Autodesk tools are their go- to solution. 1

2 Learn How To Speed Up Fusion 360 Workflows 1. Open local neutral files Have a neutral file on your computer you want to open in Fusion 360? Instead of uploading it, simply create a new Fusion 360 design from that file! From the File menu in Fusion 360, select New Design From File. The following file formats can be opened immediately:.f3d,.igs,.iges,.sat,.smt,.stp,.step 2. Replace appearances by dragging and dropping Have an appearance applied to multiple bodies and faces and want to quickly swap it out for an entirely different appearance? Instead of dragging and dropping a new appearance onto each body and face, simply drag and drop the new appearance on top of the existing swatch! 3. Make direct sketch changes for dynamic edits Have sketch geometry that isn t fully constrained? Outside of the sketch, you re still able to click and drag on geometry to move it, or change its size, making dynamic design changes. You ll see how much faster this is than editing and stopping a sketch every time you want to make a change! 2

3 This can be really useful during the early design stages. After determining the sketch geometry location/size I like, I ll often go back and add a dimension to the sketch geometry to lock it in. 4. Utilize User Parameters to control multiple features Find yourself having a handful of parameters that appear throughout multiple features in your Design? Utilize the parametric capabilities of Fusion 360 to create a single User Parameter that drives multiple features. To create a new User Parameter, first choose Modify > Change Parameters to open the parameters window. Next, Click the green + icon to create your user parameter. Give it a name, expression, and units, and then simply use this parameter name in any other feature. Change your User Parameter s expression, and all other features referencing that parameter will update automatically. 5. Automate cloud renderings with Named Views Did you know that Fusion 360 can create a cloud rendering from any of the Named (Top, Front, Right, and Home) Views with each new version saved? In addition, it s possible to create a new Named View that will be added to the list of views automatically rendered. To create a new Named View - maybe a particular angle of your product that you love first orbit around the model and zoom until you have the perfect view. With the view set, right click on the Named Views folder in the Browser and choose New Named View. 3

4 You ll now have a new Named View that you can quickly move to by simply clicking on it in the Browser. Next, to choose the views that are automatically rendered on the cloud with each save, we ll switch to the Render workspace. Click on your current workspace in the upper- left and choose Render. At the bottom of the screen you ll see the Rendering Gallery (you might have to expand it). Pick any Named View that you want to render with each save, and drag it into the Render on Save Section. 6. Promote an old version from the Data Panel Make a few saves to a design and want to quickly revert back to an older version? No need to jump to A360 promote a particular version of your design from within the Data Panel. To do this, navigate to the design you wish to update in the Data Panel and click the icon. Next, choose Click here to see versions, and a list of versions will appear. Find the version you d like to promote, select it, and lastly choose the Promote icon. 4

5 7. Utilize the S Key to quickly find any Command Tired of navigating through the various menus at the top Ribbon? With the November release of Fusion 360, there is now a shortcut just for you. In any workspace, simply hit the S key to open the command toolbox. Inside of this toolbox, you can search for any command. To choose a command, either click it or use the arrow keys and press enter. In addition to searching, you can pin commands to the top section of the Toolbox for any given workspace. To do this, search for the command you wish to pin and click the up- arrow icon. Learn How to Easily Make Selections 8. Easily select Joint Origins Ever have a hard time selecting that one Joint Origin in the middle of a complex assembly? Make sure you re utilizing the command ( ) and ctrl keys! When selecting a Joint Origin, move your mouse until you can see the Joint Origin you d like to select. With the Joint Origin displayed, hold command (Mac) or ctrl (PC) to lock in the currently displayed Joint Origins. While holding down command / ctrl key, make your selection. Easy! 5

6 9. Add or remove from a selection within a Feature Ever find yourself in the middle of a command and feel like you can t add to or remove from the selections you ve made? Similar to the Joint Origin tip above, the command or ctrl key will save you some serious time. Instead of canceling the command and re- selecting your geometry, simply hold command (Mac) or ctrl (PC) and change your selection! This tip works for all commands, from fillets to extrusions. 10. Add faces to the selection of the Shell command Similar to the tip above, it s possible to remove multiple faces with the Shell command, while still maintaining uniform wall thickness. Selecting a body from the Browser for the Shell command will hollow out the entire part (like an Easter egg), where selecting a face will remove that face and shell out the remaining form. The trick to input multiple faces for the Shell command is (again) the command on Mac, and the ctrl key on PC. Hold the appropriate key down and select multiple faces to remove! 11. Select something hidden behind other objects Working in a 3D tool on a 2D screen, there comes a time when the object you want to select is hidden behind other pieces of geometry. In Fusion 360, there s one quick tip for making these selections in between layered objects a breeze. To select an object that is difficult to select, simply left- click and hold with your cursor on top of the geometry you want to select. Next, you ll see a list of possible objects to select. Let go of the left- click, and simply choose the piece of geometry you like! 6

7 12. Utilize Selection Sets to group objects Find yourself repeatedly selecting the same components, edges, or bodies in Fusion 360? Save time by utilizing selection sets for those pesky selections! Selection Sets allow you to group multiple objects and select them at any time with a single click. To create a selection set, first select all of the objects you wish to group. If you re selecting a long list of components from your Browser, be sure to leverage the shift key to select a range of components. With your objects selected, right- click on any of the select components, and choose Create Selection Set. Now, towards the top of your Browser you ll see a selection set with a simple Select button. Whenever you want to select all objects in the Selection set, simply click Select. With your objects selected, you can right- click anywhere to perform batch operations to the selected objects, such as Show/Hide! Learn Important Best Practices and Hard- to- Find Tricks 13. Quickly change a component s opacity Need to quickly see through a component in Fusion 360? Instead of applying a transparent appearance, or switching to wireframe mode (what year is it, 1984?), utilize the ability to set a component s Opacity! To do this, right- click on a component in the Browser and select Opacity Control. In the Opacity Control dialog window, simply set the opacity that you like. 7

8 14. Turn the parametric timeline on for an imported file By default, when you import a part into Fusion 360, the parametric timeline is turned off. This is so you can make quick direct changes to the model without worrying about maintaining parametric history. But what if you want to capture your features in Fusion 360 from that point moving forward? Simply turn the parametric timeline on! To do this, right- click on the very top level of the browser (the imported part s name) and choose Capture Design History. Even though the imported model was built outside of Fusion 360, all subsequent features will be added to the parametric timeline. 15. Edit an appearance swatch Did you know you can easily edit any appearance in Fusion 360? Don t like the default blue for Matte Plastic Blue? With a few simple clicks, you can edit it to the exact color (yes, even RGB value) that you want! To start, open the appearance dialog window by choosing Modify > Appearance, or by using the A hotkey. Next, right- click on the appearance swatch you wish to edit, and select Edit. In the next window, you ll see you can pick from a wide variety of colors with the slider at the top, and crosshair within the color picker. Is the appearance too glossy? Simply increase the Roughness! You can even re- name your new appearance by editing the text field at the top of the Edit Appearance window. 16. Customize important preferences Don t like the default appearance of parts in Fusion 360, or want to have the Z- axis point up? There are a handful of preferences in Fusion 360 that can truly make you feel at home. The first thing we ll do is open up the Preferences window by clicking on our name in the upper- right corner and choosing Preferences. Starting in the General tab, we ll see that we can change the default modeling orientation from Y up to Z up. If you find yourself constantly flipping parts after bringing them into your 3D Printing slicer, this will fix that issue. 8

9 Next, in the Design tab, we can change the Default Workspace. Personally, I prefer the default workspace to be Model, so when I import parts into Fusion 360, I have my modeling tools ready to go (instead of Sculpt). Lastly, in the Material tab, we can check the box for Apply a different appearance to change the default look of parts in Fusion 360. I prefer a more matte look to my parts, so I ve set my default appearance to an Opaque Matte Gray Plastic! 17. Improve T- Spline performance with Box Mode If you ever have a hard time making that T- Spline body with perfect topology, or want to make the sculpting performance even better, Box Mode is just for you. In Fusion 360, when you re sculpting a T- Spline form, there are three view modes: Smooth mode (default) shows the actual model, Box mode displays only the control framework, and Control frame mode displays the framework and the actual model. To turn a T- Spline form into Box Mode, first select at least one face. Next, hold control (Mac) or Alt (PC) and press 1 for Box mode. You ll now see the control framework, making it easier to refine the topology and discover any accidental self- intersections. You ll also notice an improvement in performance; alt- extruding will be much, much faster. To return to Smooth mode, select at least one face and hold control (Mac) or Alt (PC) and press 3. Additionally, control/alt + 2 will enable control frame mode. Smooth Mode Box Mode 9

10 18. Add Control Points to a Spline Drawn a Spline, only to realize that you need to add an additional Control Point? No need to throw away all that work and delete the Spline - use this quick tip to add Control Points wherever you like. First, left- click and select the Spline you d like to edit. Next, right- click and choose Insert Spline Fit Point. Lastly, left- click anywhere on the existing Spline to add your new control point! Now you can add that extra change in curvature you ve always wanted. 19. Apply Sketch relationships with a right- click Find yourself repeatedly selecting sketch geometry to constrain, and navigating to the Sketch Palette on the right- hand side to pick the constraint? With a simple right- click, you can save some serious time and mouse movement. As you normally would, select the sketch geometry you d like to constrain. Next, right- click to bring up the marking menu. Towards the bottom of the menu, you ll see a list of possible constraints to choose from. Choose the constraint you like, and you re off and running. One thing to note is that Fusion 360 will intelligently display appropriate constraints based on your selection. 10

11 20. Leverage Distributed Design options Want to import one design into another in Fusion 360? Make sure you re taking advantage of all of the Distributed Design options! Starting with the basics, to insert a Fusion 360 design into another one, open the design for which you ll be insert into. Next, within the Data Panel, navigate to the design that you would like to insert. Right- click on the design and choose Insert into Current Design. Now with the linked design inserted, we can take a look at all of the version management options that we have. The link icon next to the inserted component denotes that it is linked to its original design file, and that any changes to the original design will trigger a notification. For an out- of- date component, the most common step is to update it to the most recent versoin. To do this, right- click on the out- of- date component and choose Get Latest. Now what if we don t want to update to the latest version, but instead want to choose a particular version. To do this, right- click on the out- of- date component and click Choose Version. Next, a dialog window will appear where you can select the specific version to use. 11

12 Lastly, what if we don t want the inserted component to be linked to the original one? Maybe we ve taken the original design in a different direction and don t want to bother with the notifications. From the same right- click menu, choose Break Link. 12