Fusion 360 Parameters: A Sheet Goods Reference

I keep one cabinet in Fusion and I refuse to redraw it. New width, new height, new shelf count. I change the number and the sketches follow.

The fingers do not follow. A parameter is a number with a name. The joint is still a stack of sketches, and Fusion will not rebuild that stack because you edited Thickness.

This is the sheet I wish I had taped to the monitor. How the expressions parse, how to fake an if, and which dimension goes quiet on you.

A name, a value, a unit

cabinet_width = 24 in. Anything in the model that uses that name updates when the value changes.

Fusion keeps two lists.

Model parameters appear every time you type a dimension. They come out as d17. The sketch is happy. Six months later you will not know which one is the shelf.

User parameters are the ones you name yourself in the parameters dialog. Thickness, kerf, the overall box. Make those first, then point the sketch dimensions at them.

One cabinet, cut once: skip it. You will spend longer naming things than building the box.

The same cabinet in three widths: name the numbers before you sketch the second one.

The window

Modify > Change Parameters, or the parameters icon at the bottom of the canvas, next to the timeline. Same dialog. User parameters, then favorites, then the model parameters Fusion made for you.

Name them before the first line.

• Thickness
• Kerf
• Width, Height, Depth
• ShelfCount
• Reveal, when a door or a drawer front needs a gap

Fusion sorts alphabetically, so Depth lands above Thickness for no reason that matters in the shop. A number prefix fixes the order: 01_Thickness, 02_Kerf. The list then reads the way you build.

Units go in the value. Thickness can hold 18 mm or 3/4 in. Every joint reads that one number.

Start a name with an underscore and Fusion hides it. I use that for scratch math I do not want to scroll past. Write the name down. The dialog will not remind you.

Star the two or three values you change per job. They show up under favorites. Past a dozen user parameters, split the design into components and let each one keep its own sketches. A long list is how the wrong width gets edited.

Expressions

The result has to carry a unit.

shelfWidth / 2 is fine. shelfWidth / 2 + 5 fails. Write 5 mm or 5 in.

Call another parameter by name: cabinetHeight - 2 * t, where t is the plywood.

1 in, 12 mm, and 2.54 cm can sit in the same expression. Fusion converts them when it evaluates. A unitless number becomes a length if you write shelfGap * 1 mm.

Function	What you get	Where I use it
floor(x)	Rounds down	Finger count, shelf count
ceil(x)	Rounds up	At least this many shelves
min(a; b)	The smaller one	Cap a finger or a gap
max(a; b)	The larger one	Keep a finger above a minimum
sqrt(x)	Square root	A brace across a corner
abs(x)	Drops the sign	Kerf math that went negative

Semicolon between arguments. A comma throws a parse error that looks like a bad name.

Shelves from the cabinet height

Top, bottom, and every shelf consume thickness. The openings are one more than the number of shelves.

t = 3/4 in
cabinetHeight = 48 in
openingTarget = 10 in
shelfCount = floor( (cabinetHeight - 2 * t - openingTarget) / (openingTarget + t) )
shelfSpacing = (cabinetHeight - (shelfCount + 2) * t) / (shelfCount + 1)

The first opening costs you openingTarget. Each shelf after that costs another opening plus one thickness. shelfSpacing is whatever is left after the top, the bottom, and those shelves take their 3/4.

Those numbers give 3 shelves and openings of 11.0625 in. Set cabinetHeight to 60 in and the same lines give 4 shelves at 11.1 in. You type a height. You do not redraw the shelves.

If shelfCount comes back 0, you have a box with no shelf, and shelfSpacing is the inside height. That is the formula doing the right thing.

There is no if

You cannot write "6 mm ply gets 3 mm fingers, 18 mm gets something wider." The expression engine has no if/then.

sign() returns 1, 0, or -1. sign(thickness - 12 mm) is positive, dead on the cutoff, or negative. Zero is its own answer. It is not a no.

min and max clamp. Half the thickness, held between 3 mm and 6 mm:

fingerWidth = max(3 mm; min(6 mm; thickness / 2))

To pick A when x is positive and B when it is negative:

(sign(x) + 1) / 2 * A + (1 - sign(x)) / 2 * B

On exactly zero that returns the average of A and B. Keep the test off zero if an average finger is nonsense.

I stop there. One more nest of sign and min and the line is a puzzle, and a typo takes the model with it. A parameter can pick a width. It still will not decide which tabs exist, or which slot they meet.

It updated everything except the one edge

You inserted a component and the parameters are gone. They live in the file where you named them. Bring another design's parts into the cabinet and the names stay behind, unless that insert dialog offered to bring parameters and you took the offer. Otherwise type the list again.

The dimension shows a number and no fx. It was never driven by a parameter. Later edits skip it. No warning. The rest of the model moves and that one edge stays. Click the dimension and type the name.

A typo does not error. Fusion creates a new user parameter under the misspelling and drives the dimension from that. You now have thikness and thickness. Check the list before you trust the sketch.

Yellow warning in the parameters window. Something references itself, sometimes through a second parameter. Updates stop. Point one expression at a plain value and the loop breaks.

The model is just dead. Roll the timeline marker back to the first sketch. Check each dimension. Step forward one feature at a time until one fails to compute. It is usually a sketch you dimensioned by hand months ago. Relink that dimension. Leave the rest of the cabinet up.

A key, if you want one

There is no default shortcut. Press s, type Change Parameters, and bind it. I use p.

In the window, double-click a value and edit it there. Tab moves down the list. Width, depth, and height at the top, and a resize is a few seconds.

You can do this from inside a sketch. Type the dimension, then the name: cab_width - 19 mm. Fusion reads the user parameters you already saved. Spell it the way it is spelled. A misspelling becomes a new parameter, same as above.

Save the list

Build one cabinet the long way. Save a copy. Strip it back to a dummy box and the parameters. The list I keep:

• Sheet thickness
• Kerf
• Inside width, inside height, inside depth
• A panel thickness override, for when the back is thinner
• Back inset
• Drawer front gap
• Shelf-hole spacing
• Divider spacing

Drive the sketches from those. Save the file as a template. The next job starts with the names already hooked up.

If you would rather start from a box that already has joints, open one from the gallery, change the size, and export.

The joint is a different job

Parameters will change the cabinet all afternoon. The fingers are still sketches you patterned by hand. Go from 6 mm ply to 18 mm and you draw that joint again. The parameter changed a number.

Boxes.py will generate a laser-cut box, and plenty of shops stop there. Kerf is one number. It will not take a different kerf in X and in Y. MakerCase is the fast path for a plain finger-joint box, and it stays on plain boxes. PanelOrca lays parts out on a sheet. Fusion will let you model anything, and you will model the joint yourself.

GCrafter treats the joint as part of the design. You set the box, pick the joint, change a dimension, and the fingers come with it, including a separate kerf for X and for Y. That split is the one people still cannot get out of LCInterlocking on the LightBurn forum. This is sheet-goods joinery. A sculpted chair back still belongs in Fusion.

FAQ

Can you use if/then in a Fusion 360 parameter?

No. sign, min, and max are the workaround. max(3 mm; min(6 mm; thickness / 2)) holds a finger width between 3 mm and 6 mm. There is no if.

A parameter disappeared.

Open Modify > Change Parameters and look for the yellow warning. That is usually a parameter referring to itself. If the name vanished after an insert, it is still in the other file. If the model simply stopped moving, roll the timeline to the first sketch and find the dimension with no fx icon.

What units, if I work in inches?

Put the unit in the value. Thickness can be 3/4 in or 18 mm. A bare + 5 fails. + 5 mm works, including inside an expression that is otherwise in inches. Fusion converts the literal.

Do sketches update on their own?

The dimensions that actually point at a parameter do. A plain number with no fx icon sits there forever. Click it, type the name, and check the parameters list so you did not just invent a typo. Most dead cabinets are that one dimension.

Can I copy user parameters into another design?

Not by inserting the components. The names stay in the source file unless the insert option says it will bring them. The reliable version is the template: new job, the list is already there.

Happy making.

Andy