Parameters in Parametric Models

Naming Scheme

Something I've learned the hard way is that you need to have a naming scheme when you start to do a lot of parameters in your models. Otherwise, you end up finding it difficult to identify which parameter you're looking for. Parameters in Fusion360 can have alphanumeric characters and the following special characters:

• _ Underscore
• " Double Quote
• $ Dollar symbol
• ° Degree symbol
• µ Micro symbol

They cannot have a space, so I typically use PascalCase. This is the scheme I use:

In addition, I always create the following three parameters to allow for modeling of various types of fit if something is going to be 3D printed.

Calculations

Starting with the May 2023 release of Fusion360, you can now use conditional operations in your parameters. This is covered in the reference. This opens up a huge new arena for exploration. For example, you could do something (simplified) like this for the number of holes in a hub:

HoleCount = if(HubOD >= 100mm; 7; 5)

This would set the HoleCount to 7 if the HubOD (hub outer diameter) is greater than or equal to 100mm. You can also chain them together:

HoleCount = if(HubOD >= 100mm; if(HubOD >= 200mm; 9; 7); 5)

Default User Parameters

One of the most powerful things with a parametric modeling tool is being able to create standard parameters that drive the model. Often, a lot of these are references to external parts that you need to interact with, like a screw. To simplify my life, I have put together a CSV that contains:

• Fits for my printer: interference, transitional, and clearance.
• Standard metric screws for M2 - M12 in all the default standard threads. This is for socket head screws, which are my go-to. The insert and tap information will work for any metric screw of that size and thread pitch (yay metric!). These are all just "standard" thread pitches.
• Sizes for threaded inserts.

You can download the CSV from here: f360_default_parameters.csv

You can import them quickly with the Parameters I/O add-on that Autodesk provides (you'll need to install for some weird reason). Once imported, if you look at user parameters, you'll see something like this:

The naming is based on this pattern:

• <type of fit>Fit<layer height without decimal> for the various fits.
• <size>Head<OD/Depth> for the outside diameter (OD) and depth (height) of the screw.
• <size>InsertHoleID for the inside diameter (ID) of the hole you'll need to insert the insert.
• <size>InsertDepth for the depth of the insert when you do an extrude cut. Note there are also some InsertShortDepth for the CNC Kitchen short inserts.
• <size>TapeHoleID for the ID of the hole you'll need if you plan on tapping the holes.
• <size><fit>ClearanceHoleID for the clearance holes as specified in Machinery's Handbook in their normal, close, and loose fits.

I've provided references to where the data came from originally (for example, the McMaster-Carr screw part numbers). There's a few things you might need to do:

1. You should update the fits for your printer. This is just for my Prusa MINI+, and won't necessarily match yours. It's a good start if you don't want to fuss about it, although many cheap 3D printers have much bigger tolerances.
2. When you want to use M3HeadOD (for example), you'll want to allow for tolerance. I typically use TransitionFit030, which will get a snug fit that doesn't drag when you put the screw in. To do that, when you create the circle, just set the size to M3HeadOD + TransitionFit030. I didn't include the fit in the main size because different people want different fits in different situations.