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 hitting 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 make this name T for thickness, and change the expression to 15.
%20(1).png)
Learn CAD
- Nationally accredited
- Create your own portfolio
- Free student software
- Learn at your convenience
- Authorized Autodesk training center
You can see my units have been automatically set at millimeters. In the comment, I will change this to 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 name it with a larger name.
I'll hit OK, and let's create a couple more parameters. I will name this W for width, and I will make this expression 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, and make this 5, and I'll change this to Whole Diameter. I will add one more parameter just to show an example.
If I named this Part Width, and made this expression 30, just like our width is 30, and named this Part Width, and hit OK, let's see what happens when I try to enter one of my parameters. Leave this in for now. We'll delete it in a minute.
I'll go 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 up to Sketch, Rectangle, Center Rectangle. I'll place the center point here, and make my rectangle like this. D for dimension, and I'll dimension this 235 × 125.
I would like to create another rectangle here, so I will go Sketch, Rectangle, Center Rectangle, and create my rectangle like this. D for dimension, and here is where we will begin to use our user parameters. I want this to be the width of my part, or 30, so I will type in W. We can see that Part Width and W both appear, because that is in their name.
For now, hit W, and 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 change this parameter, so I will start typing in T for thickness. You will see that Part Width also appears as one of my options, because T is found somewhere in its name.
If I name all of my parameters with long names, because the word width involves a T and a W and a D, all of those names will bring up this parameter as a suggested parameter. By keeping them as one or two letters, only the expected parameters will appear. So go T, Enter, and you will see FX 15.
Let's now place a horizontal-vertical constraint between the two center points of my rectangles. I will go D one more time, and place a dimension between these lines. Here, I do not want to do the width parameter.
I want to actually type 30. This is a static value, and I do not want it to update as I update my parts. I will go ahead and hit Stop Sketch, and return to my Home View.
Before we go any further, I am going to go Modify, Change Parameters, and delete the Part Width parameter by hitting this X. Now, by looking at this rectangle here, we can see how the user parameters update our model. If I go to my thickness and type in 12.5, we will see that rectangle grow shorter. And if I type here 40, we will see that rectangle grow wider.
Everything in my model that is referenced by these parameters will automatically update as I update the expression in this window. I will return these to 30 and 15, and we will be editing and checking these parameters as we build our model. This is a good way to make sure our model remains parametric and updates the way we expect it to.
I will go OK, hit the Home View, and save my model. In the next video, we will finish our base component by using user parameters. I will see you in the next video.
