Discover how user parameters in Fusion 360 can drive the creation and modification of your models. Learn the step-by-step process of setting up, using and modifying user parameters to ensure your models remain parametric and adapt as expected.
Key Insights
- User parameters in Fusion 360 let you assign specific values to parameters, which can be utilized instead of a number for a dimension or feature in your model. This leads to automatic updates of the model as user parameters are modified.
- Creating a user parameter involves defining a short name, setting an expression value, and adding a descriptor comment. Keeping the parameter name short (one to two letters max) ensures only expected parameters appear when making adjustments.
- The use of user parameters allows for a dynamic modeling process where changes in parameter values automatically result in corresponding changes in the model. This capability facilitates a more efficient model updating process.
In this video, we will begin to build our base, but first I would like to take a look at building user parameters. You can see that I am in my Fusion 102 Parametric Modeling folder, and let's open Step 1: Base.
This file does not have any components or geometry inside of it, but we are using this file to set up some of our preferences, including material and units. Once your file is open, go ahead and hide your data panel. So let's take a few minutes to look at user parameters in Fusion 360.
If I go to Modify > Change Parameters, it will bring up this dialog box, which will show us our user parameters. You can see that I do not have any parameters made in this model yet. We will make them in a minute.
User parameters allow us to assign values to specific parameters, and these will automatically be referenced by our model if we input them instead of a number for a dimension or other feature. This allows us to edit our user parameters, and the model itself will automatically update with those new part thicknesses, widths, hole diameters, or whatever you use for your user parameter. So let's create some user parameters now.
You can create a parameter by clicking the plus sign right here. The Add User Parameter window will open, and you will see some boxes that we need to fill out. I will name this parameter T for thickness, and change the expression to 15.
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You can see my units have been automatically set to millimeters. In the comment, I will type “Part Thickness” so that I can remember what the T stands for. I like to leave the name of my parameter short—one or two letters at most—because in a minute, I will show you what happens when we use longer names.
I’ll click OK, and let's create a couple more parameters. I will name this W for width, and I will set the expression to 30. Remember, the expression value can change as we update our parameters, but I will be starting with a width of 30.
Let's add one more. I’ll name this D, make it 5, and in the comment write “Hole Diameter.” I will add one more parameter just as an example.
If I name this one “Part Width” and make the expression 30—just like our W parameter—and then click OK, let’s see what happens when I try to enter one of these parameters. Leave this one in for now. We’ll delete it in a minute.
I’ll click OK, and now we can begin to create our model. I’ll right-click > New Component, and rename this component “Base.” With our new component active, I’ll create a sketch and host it to the bottom plane.
Now let's go to Sketch > Rectangle > Center Rectangle. I’ll place the center point here and draw the rectangle. Then, press D for Dimension, and I’ll dimension this to 235 × 125.
I would like to create another rectangle here, so I’ll go to Sketch > Rectangle > Center Rectangle and draw the shape. Press D for Dimension, and here’s where we’ll begin using our user parameters. I want this to be the width of my part—or 30—so I will type in W. You’ll see that “Part Width” and “W” both appear because that character is found in both parameter names.
For now, select W and press ENTER. We can see that Fusion has now inferred a function for the dimension—it says “Function: 30.”
I can change this function, and we will do so in the next video. Now I want to apply the thickness parameter, so I will start typing T for thickness. You’ll notice that “Part Width” also appears as one of the suggestions because T is found in its name.
If I name all of my parameters with long names, parameters like “Width” and “Diameter” may bring up other unintended matches. By keeping them to one or two letters, only the expected parameters will appear. So I’ll go T, press ENTER, and you will see “fx: 15.”
Now let’s place a Horizontal/Vertical constraint between the two center points of my rectangles. I’ll press D one more time and place a dimension between these lines. Here, I do not want to use a parameter.
I want to manually type 30. This is a static value, and I do not want it to update as I update my parts. I’ll go ahead and click Stop Sketch and return to my Home view.
Before we go any further, I’m going to go to Modify > Change Parameters and delete the “Part Width” parameter by clicking the X. Now, by looking at this rectangle here, we can see how the user parameters update our model. If I change the thickness to 12.5, we will see the rectangle get shorter. And if I change the width to 40, we’ll see the rectangle grow wider.
Everything in my model that is referenced by these parameters will automatically update when I change the expression in this window. I will return these to 30 and 15, and we will continue editing and checking these parameters as we build the model. This is a good way to ensure our model remains parametric and updates the way we expect it to.
I will click OK, return to the Home view, and save the model. In the next video, we will finish our base component by using user parameters. I’ll see you in the next video.
