Fusion 360 parameter tables

I keep the numbers that drive a design — wall thickness, box size, the clearance for a lid — as user parameters in Fusion. Typing twenty of them into the Change Parameters dialog one at a time is slow, and Fusion only tells you an expression is wrong after you’ve typed it. This page is a table to build them in, with the expressions checked as you type, and a file Fusion imports in one go.

How to use it

Add parameters (or Sample for a small box, or Import CSV for one exported from Fusion). Each has a name, a unit, an expression and a comment; tick ★ to make it a favourite (it shows at the top of Fusion’s dialog). The value column shows the result in the parameter’s unit, and any error underneath.
Expressions follow Fusion’s syntax:
- numbers with units — 80 mm, 3.2in, 1.5 deg, 2 mm * 3 mm (an area); other parameters by name; + - * / % ^ and brackets; PI, E;
- functions with their arguments separated by ; (not ,): sin, cos, tan (angles), asin, acos, atan, sqrt, abs, sign, exp, ln, log, floor, ceil, round (unitless — write floor(width / 1 mm)), max(a; b), min(a; b), pow(a; b);
- comparisons > < >= ⇐ == <> with if(test; then; else), and(…), or(…), not(…). Units are checked: a length plus an angle is an error, a result in mm² can’t go in a mm parameter. A number with no unit next to a length takes the document unit (as Fusion does), and the note says so. Names follow Fusion’s rules (a letter first, no spaces); d1, d2… get a warning because Fusion uses them for its own model parameters. Circular references and unknown names are caught.
Configurations: tick the parameters that vary, add a row a variant and type the expressions that differ (empty keeps the default). Each cell shows the value it gives, and Values of the other parameters shows what the derived ones come out as in each variant. Copy as a table puts it on the clipboard tab-separated for pasting into Fusion’s configuration table.
Fits and clearances: pick a process and a fit, give a nominal diameter and a name prefix, and Add as parameters adds the nominal, the hole and the shaft (or the clearance) as parameters that refer to each other. Machined parts use ISO 286 hole-basis fits — H11/c11 loose running down to H7/p6 press — with the limits shown and the sizes modelled at the middle of each band. Printed parts use the clearances from print tolerances for FDM, resin and SLS (print its clearance test to tune them to your printer).
Export the default values or one configuration, in one of three forms:
- Change Parameters CSV — Fusion’s own format: Modify → Change Parameters → Import. A header row Name,Unit,Expression,Value,Comments,Favorite, then one row a parameter (Value in the parameter’s unit, Favorite TRUE/FALSE), UTF-8. This is the file Fusion’s Export in the same dialog writes, so you can also import one here, edit it and send it back. The import dialog lets you untick rows.
- ParameterIO CSV — for Autodesk’s ParameterIO sample add-in (and the scripts based on it): no header row, then name, unit, expression, comment. It adds new names and updates existing ones.
- Python script — a Fusion script (Utilities → Scripts and Add-Ins → Create) that adds or updates each parameter through the API (userParameters.add / .expression), for any Fusion version. Parameters are written with each one after those it uses, so an importer that adds them in order never meets a name it doesn’t know yet. One CSV a configuration downloads a file for each variant.

The table is kept in this browser; Share makes a link that carries it.

What it doesn’t do

The evaluator covers what people put in parameters, not every corner of Fusion’s: text parameters, random() beyond a number, and the less common units are not checked. Fusion is the final word — if it rejects an expression this page accepts, tell me.

Privacy

Nothing leaves your browser. The fit tables load from this site (the print tolerance tool’s script).