Join Thom Tremblay for an in-depth discussion in this video Setting up parameters, part of Fusion 360: Designing for Metal.
- [Instructor] Every dimension added to a sketch, and every value used to define a feature has a name given to it. In this video, we will see that an easy way to improve you ability to quickly edit multiple features in Fusion 360 is to edit the parameters directly. Going to my project where I've uploaded the data, I'm going to open the 01-01 file. Once the file is open, I'll hide the Data panel to restore the screen space. I can see that all I have presently in this design is the sketch.
That sketch is created directly under the top level of the design, and is the only item in the timeline. To edit the sketch, I can double-click the icon in the timeline. When it opens, the sketch will show me all of the dimensions that are used to define it. Some of these dimensions carry an extra symbol that shows that they are related to others. And, you'll see that some of the lines have a different coloration showing that they are presently under-constrained.
The first thing that I'd like to do is go ahead and completely constrain the sketch by adding the dimension that will define the thickness of this feature. I'll start the sketch dimension tool, select the lines, and when I go to place the dimension what I want to do is, rather than typing in a value, I want to relate it to the thickness of the wall of the o-clamp. So, I'll select the dimension that presently defines it. When I do, it will put the name of that dimension in as the value.
I'll press enter, and we'll update the sketch. Taking a look at another dimension, I'll see that there is a complex relationship built. D3 is divided by two, and then the value of d2 is added to it. Then, half of the value of d2 is added to that, which is great as long as I know what d3 and d2 are. If I'm new to this sketch and I don't understand why this dimension would be defined this way, it's very hard to understand the design-thinking behind it.
A great way to make these relationships make more sense is to apply real names to the dimensions. To do this, I'll go under the Modify pull-down and use the change parameters tool. This will show me a list of all of the dimensions of all the sketches, and, if I had 3D features, the heights of any extrusions, the radius of any fillets, and it even gives me a nice detailed description of what that dimension is applied to. If I bring the dialog down, I can start to relate things.
For example, this 36 millimeter dimension relates to the inner diameter of the o-clamp. The 1.5 millimeter dimension relates to the wall thickness. So, let's change the names automatically generated by Fusion 360 and give them more meaning, such as, inner diameter. These values are case-sensitive, and you must spell them correctly if you want to reuse them, or relate them to other dimensions. While we're here, we can change the value for the pin diameter as well.
With these updated, let's return back to the sketch and now edit this dimension. Now, I can see that the pin diameter is divided by two with the wall thickness and half of the wall thickness, again, added to it. That's how this dimension is calculated. There are times where we might want to create a parameter ahead of time before we have anything to define with it. If I return back to change parameters, I can create a user parameter, give it a name, select the units to use, there's a wide variety for a number of different purposes.
We can also use no units if we want to setup the number of instances in a pattern, or something related to that. We can enter the value of the expression. In this case, it would be 20 millimeters. And, even enter a comment. Now that parameter is ready and waiting for me if I ever decide to use it. I can also make modifications to the values of the parameters from the dialog. For example, if I change the diameter value from 36 to 39, you'll see the sketch automatically updates.
If I change the wall thickness from 1.5 to three millimeters, it, too, updates, and everything related to it in the sketch is kept up-to-date. When elements of your design rely on or have relationships to other elements, it's worth taking just a few minutes to define.
- Setting up parameters
- Joining components
- Animating and rendering the design
- Testing alternative materials
- Creating the setup
- Publishing and posting the design