Discover the intricacies of setting up user preferences, sketch-based modeling, and workspace configuration for building a lamp design on Fusion software. Master the techniques of setting units, materials, visual style, creating components, sketching, dimensioning, constraining, and extruding in this comprehensive guide.
Key Insights
- The user preferences can be customised in Fusion software to suit the requirements of the design, including setting units to millimeters, material to wood and pine, and modifying the pan-zoom-orbit shortcuts.
- Sketch-based modeling involves creating a new component for the model, renaming it, and ensuring that new geometry is created in this component. The sketch toolbar is used for creating sketches and assigning specific dimensions.
- Workspace configuration includes setting up visual styles, environment, enabling or disabling Environmental Dome and Ground Plane, and setting the camera to Orthographic. The last step involves extruding the geometry and saving the file.
In this video, we will set up our user preferences and use sketch-based modeling to start building our lamp. I will go over into my Data Panel and open Step 01, Base, by double-clicking.
Once my file is open, I can hit the X or the grid to hide my Data Panel. If we go up to where our name is shown here and go to Preferences, we can see what preferences opening this file has automatically set up. If I go to Units in Design, CAM, and Simulation, we will see that they are set to millimeters.
And if I go to Material, we will see that it is set to Wood and Pine. Because most of the parts we will be building for this lamp are going to be made out of wood, it is good to show this when we are modeling. The default for Fusion is Metal.
If we go to General, we can see that we have a Y-Up default modeling orientation, and my Pan-Zoom-Orbit shortcuts are set to Fusion and Constrained Orbit. Also, you may want to check Reverse Zoom Direction if you are used to zooming the opposite way that Fusion, Inventor, and SolidWorks zoom. I will hit OK.
And let's continue to set up our workspace. You will notice that I have turned off my grid, and that is down here at the bottom under Grid and Snaps. My Layout Grid is off, and this is for the video to make it more clear.
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I have also unchecked Snap to Grid and Incremental Move. You may feel free to keep these on, but we have found that it is more clear to record with them off. Also, under Display Settings, my visual style is set to Shaded with Visible Edges.
My environment is the Photo Booth environment. I have my Environmental Dome and Ground Plane off, and Object Shadow and Ambient Occlusion off. Again, this is for clarity when recording the video, but you may set these settings on or off, depending on what you prefer.
Finally, my camera is set to Orthographic, although when I am working, I tend to work in perspective with ortho faces. So let's begin modeling. The first thing I would like to do is to make a new component for my model.
Rule Number One in Fusion is to always build your geometry in a component. Rule Number Two is to always rename your component. Under the Assemble tab, we can see the New Component icon.
When I click this, a new component will be made in my model. I will rename this Base, and I will say that it is an empty component, and I will have the Activate checkbox checked. When I hit OK, we will see in our browser a new component is made, and this radio button to the right is showing that it is my Active Component.
This means that whenever new geometry is created, it will be created in this component. So let's begin by creating our first sketch. This icon here under the Sketch toolbar is Create Sketch.
I will click the icon, and you will see our origin planes and axes appear. We can select any plane for our sketch creation, and I will hover over the bottom portion of my screen to select the plane perpendicular to my Y-axis or along the Z and X-axes. My view will automatically reorient itself to be facing the XZ plane, and I can begin creating my sketch.
Let's go back to the Sketch toolbar and select Two-Point Rectangle. I will create a rectangle, and I will just click twice here at the bottom of my screen. You do not need to worry about specific dimensions or placing it anywhere specifically on your screen.
We are going to constrain and dimension our rectangle now. Sketch dimensions can be found under the Sketch > Sketch Dimension menu, or by hitting D on your keyboard or clicking the arrow here to add it to the toolbar. When I am working in Fusion in these videos, I will be hitting D on my keyboard to activate the Sketch Dimension.
So hit D on your keyboard, and you will see the sketch icon appear next to your cursor. I will select this line with a single click and move my mouse away from the line to dimension. Click again to place your dimension, and then type in your distance.
This will be 125 millimeters, and I will hit ENTER. I will zoom out and pan and select this line, click, move my mouse and click, and type 235 and press ENTER. For more practice with zooming and navigating in Fusion, please watch the video in Fusion Essentials.
Our sketch is now fully dimensioned, but as I click and drag on my edges, you can see that my rectangle can still move around my screen. This means that it is not yet fully constrained. In order to fully constrain it, let's go to our Sketch Palette and select a constraint.
I will go Midpoint by first hitting Escape to make sure that nothing is selected, select my Midpoint Constraint, and then click this line and click my origin point. We will now see a triangle appear next to that connection point, which is the midpoint of this line and my origin point here. Now you'll see my geometry has become black, and that means that it is fully dimensioned and constrained.
I can hit Stop Sketch in the top of my toolbar, and I will go to my ViewCube and click the Home icon to return to my Home view. The last thing we will do in this video is extrude my geometry. So let's go to the Create tab, find my Extrude tool (which is also E on the keyboard), and click this profile and drag my arrow up. I will type 15 and hit ENTER. Go ahead and save your file by hitting CTRL + S on your keyboard or clicking your Save icon here, adding your description, and clicking OK.
And in the next video, we will finish our base. I will see you in the next video.
