Join Thom Tremblay for an in-depth discussion in this video 2D drawing tools for metal, part of Fusion 360: Designing for Metal.
- [Instructor] 2D drawings have been the standard communication vehicle for mechanical design for more than a century. And they continue to be a requirement for many. Fusion 360 generates these drawings directly from the 3D model and will update the drawing as the model changes. To create a drawing inside of Fusion 360, go under the workspace fly out, go to drawing, and choose whether or not you'd like to create a drawing from the design or from the animation. We'll begin with the design.
By default, when Fusion 360 sees multiple components, it will select the full assembly option. For this video, I'd like to create a drawing just of the bottom component, for now. I'll select the bottom component. Set the standard to be ASME. I'll leave the units to be inch. And then I'd like to set the drawing size to be A size, with a landscape format. I'll click okay, and it will create the drawing sheet with the title block and a border.
And it will present me with a preview of the drawing view. I can change the orientation of the drawing view. I can change the scale, either by picking from a list of options or by typing in a specific scale. I'll set the orientation back to front. Click to place the view. And then pick okay to generate the drawing view. Looking more closely, you'll see the hidden lines created by the slot are automatically placed in the view.
Now I need to create projections. I'll start the projected view tool. Select the parent view. And place the top, left, right, and isometric view using okay to start the generation process. The views themselves maintain their orthographic projection. If I click on the base view, and move it around, you'll see that the other views follow.
Selecting a projected view, you can move it, but only within the orthographic plane. If I were to change the scale of the parent view, the orthographic projections would update, but the isometric would remain independent. In fact, I can double click on the isometric view and even change it's appearance to a shaded view, without showing tangent edges. This gives a great visual to add to your detailed drawing.
To complete the detail drawing, we need to add annotation. There are many options and while we don't have time to completely detail this drawing, let's add some of the dimensions. I'll start out with some center marks. Select the holes in one view. Choose a center mark pattern for another view. And then begin placing dimensions.
If we need a specific dimension, or want to limit the options, we can choose one of the linear, line, angular or other dimensions. Or we can use the simple dimension tool, which will create dimensions based on the selection. If I select the center of the first hole, and the center of the second hole, I can place an aligned dimension. Or by moving the mouse, I can have it generate the horizontal or the vertical dimension, depending on how I'm moving.
I'll place the dimension and begin selection other dimensions. The same rules apply. And the order in which you select geometry will determine which side the dimension value will appear on. Selecting a curved edge will give you a radius dimension. And selecting a circular edge will give you a diameter by default. Selecting an edge and then selecting an edge that is not parallel with it will also give you an angle value.
You can also simply select a single edge and place the dimension. You can continue to detail the drawing until it's complete. We also have the ability to add additional sheets to the drawing by going down to the bottom of the view and doing a quick add of another drawing sheet. On the new drawing sheet we can start the base view tool. We can either use the model as the representation, which in this case is showing the full assembly, change the scale, or change the representation to the storyboard of the animation that we want to use and place the view.
With the drawing view of the animation we have the options of applying balloons. Selecting the component will automatically generate a balloon with a unique value. And there are tools available to help us align the balloons, to clean up the drawing and improve the appearance.
We can also add a table of the parts list, which in this case shows me that I clearly have chosen the wrong sheet size, which is just fine. I don't have to start over. I merely have to go down to the sheet settings and change the sheet size and update the location of my parts list and my drawing view to clean up the drawing. The 2D drawing capabilities of Fusion 360 are already powerful, but they keep expanding and improving at a rapid pace.
If you need 2D drawings for your work, be sure to keep up to date with the upgrades to Fusion 360, and make special note of the what's new documents.
- Setting up parameters
- Joining components
- Animating and rendering the design
- Testing alternative materials
- Creating the setup
- Publishing and posting the design