Tolerance and Fit
Two parts modeled at exactly the same size will not fit together. A 10 mm peg does not go into a 10 mm hole — not in plastic, not in plywood, not ever. The gap you deliberately design in is called clearance, and choosing it on purpose is the difference between a part that assembles and a part you spend an hour sanding.
This page gives starting numbers. It does not give final numbers, because those depend on the material, the machine, and the day. The habit that actually solves fit problems is at the bottom: test the fit on a small piece first.
Why parts come out the wrong size
- 3D prints shrink and bulge. Plastic contracts as it cools, and the first layer squishes wider than the layer above it. Holes tend to come out slightly undersize; outside dimensions slightly oversize.
- A CNC bit is round and has width. It cannot cut a sharp inside corner, and the path it follows is offset by its own radius — see Designing for the CNC.
- Sheet goods aren't their nominal thickness. A sheet sold as 1/2 inch is rarely 12.7 mm. Measure the actual sheet with calipers before you model a slot for it.
Starting clearances for 3D-printed fits
Clearance here means the total gap between the two surfaces — so for a peg in a hole, split it between the two parts or take it all off one.
| You want | Start with | Example |
|---|---|---|
| Press fit — goes in hard, stays put permanently | 0 to 0.1 mm | A pin you never plan to remove |
| Snug fit — hand pressure to assemble, no wobble | about 0.2 mm | A lid, an insert, a divider |
| Free fit — moves or spins freely | 0.4 to 0.5 mm | A hinge pin, a sliding drawer |
| Around a screw or bolt shaft | 0.2 to 0.4 mm over nominal | An M3 screw through a 3.2–3.4 mm hole |
Three adjustments worth knowing:
- A print isn't solid, so you can't just drill it later. Inside those outer walls is infill — mostly air. Drilling into it gives you a ragged hole through a honeycomb, not a clean one. If a hole has to be drilled, tapped, or reamed after printing, design that region as solid material on purpose. Otherwise, model the hole and print it.
- Small holes print smaller than you drew them. Under about 5 mm diameter, add a little extra rather than planning to open it up afterward.
- Vertical holes fare better than horizontal ones. A hole printed on its side sags at the top. If a hole must be accurate, orient it vertically on the plate.
Starting clearances for CNC-cut plywood
Wood moves, splinters, and varies sheet to sheet, so the numbers are coarser than for plastic.
| You want | Start with |
|---|---|
| A tab into a slot, glued | Slot 0.1 to 0.2 mm wider than the measured tab |
| A tab into a slot, assembled dry, tight | Slot the same as the measured tab, then test |
| A shelf into a dado | Match the measured sheet thickness, not nominal |
| A printed part sitting in a routed pocket | 0.3 to 0.5 mm around it |
Always measure the actual material with calipers and model to that measurement. "1/2 inch plywood" is a name, not a dimension.
Test the fit before you commit
This is the part that matters. Before you cut or print a whole part, make a small test piece — a coupon — that has only the feature you're unsure about.
A good coupon is small, fast, and tests one thing:
- For a printed fit: a 20 mm square, 5 mm thick, with three holes in it at your three candidate clearances, labeled. Print it, try the mating part in each, and use the one that feels right. It takes a few minutes and saves a four-hour reprint.
- For a CNC joint: a short offcut with one tab and one slot at your intended dimensions. Cut it in the same material and on the same machine you'll use for the real part, since that's what you're actually calibrating.
- For a cardboard mockup: cut the full outline in cardboard on the Silhouette and hold it up against the real object it has to fit. This catches "the whole thing is 15 mm too tall" errors that no amount of clearance math will.
Record the number that worked in your journal. Next project, you start from a tested number instead of this page's guess.
When a fit is already wrong
- Too tight, plastic: sand or file it. Drilling only works if you designed that area solid — otherwise you're drilling into infill and will make a mess of it. Either way it's faster than a reprint if the part is otherwise good.
- Too tight, wood: sand the tab, not the slot — you can see what you're doing and you won't wallow out the socket.
- Too loose: shim it, or glue it. A slightly loose joint that gets glued is fine; a sloppy one, or one that has to stay removable, needs a redesign.
- Wrong by more than about a millimeter: that's not a tolerance problem, it's a measurement or units problem. Re-measure the real object and check which units your export used — see Exporting Your Design.