Tolerances & Fits

The nominal dimension is the number on the drawing - 10.00 mm. No process delivers exactly that; it delivers something within a band. Tolerance is that band, stated on purpose: the allowable deviation from nominal (say 10.00 mm plus or minus 0.1). Every real process has a characteristic tolerance - a laser cutter or a good CNC router might hold a few tenths of a millimetre, a hobby 3D printer perhaps 0.2-0.5 mm depending on axis and settings, an industrial machine far tighter - and it is set by the machine, the tool, the material and the operator together.

The professional habit is to decide which dimensions are critical and give them realistic tolerances, rather than pretending everything is exact. A shelf can be a millimetre off and nobody notices; the peg that must slide into a hole cannot. Chasing tolerance you do not need is expensive - tighter tolerances mean slower cuts, finer tools, more passes and more scrap - so good design spends precision where the fit matters and relaxes it everywhere else. 'Make it 10 mm' is not an instruction a machine can honour perfectly; 'make it 10 mm, and here is how much off it may be' is.

When two parts meet - a shaft in a hole, a tab in a slot, a pin in a bore - the relationship between their sizes is the fit, and there are three. A clearance fit leaves the hole larger than the shaft, so there is always a gap and the parts slide or turn freely; you use it for a drawer runner, a removable pin, anything that must move. An interference (press) fit makes the hole smaller than the shaft, so the parts grip and must be pressed or tapped together and stay put by friction; you use it for a dowel that should never move, a bearing seat, a permanent peg. A transition fit sits on the boundary - sometimes a whisker of clearance, sometimes a whisker of interference - giving a snug, located-but-removable joint, like a locating pin you can still pull out by hand.

What is startling the first time is how small the differences are. The gap between a part that slides, one that clicks and one that must be hammered can be two or three tenths of a millimetre - the same order of magnitude as your kerf and your machine's tolerance. That is precisely why fits and fabrication error are the same conversation: the thing that determines your fit is often the very error you have to compensate for.

Engineers formalise this with standard fit systems (for example the ISO limits-and-fits tables, where codes like H7/g6 name an exact hole-and-shaft pairing), and in precision machining you will meet that language. For most digital-fabrication work in sheet and print, you do not need the tables - you need the idea: name the fit you want, know it lives in tenths of a millimetre, and remember which way to push. The mnemonic that saves beginners is simple - for something that must move, make the hole bigger (clearance); for something that must stay, make the hole smaller (interference); for something that must locate but release, aim for the line (transition). Everything after that is finding the right number of tenths for your material and machine.

Three physical facts push the cut away from the drawn line. First, kerf and tool diameter: a laser burns a slot of finite width (the kerf, often 0.1-0.3 mm), and a router bit is a solid cylinder of, say, 6 mm. CAM offsets the toolpath to one side of your line by half that width, so the cut lands correctly if the offset is set right - but a 10 mm slot cut with the tool centred on the line comes out 6 mm too wide. Put the tool inside the line for holes and outside for parts and the nominal survives; forget, and every dimension is off by a tool radius.

Second, spring-back and material movement: plywood and MDF swell where a laser heats them and can char the edge; acrylic relaxes; metal springs back after bending; a 3D print shrinks slightly as it cools and can bulge at the first layer (elephant's foot). A laser beam is also not perfectly parallel - it focuses to a waist and then diverges, so a thick cut can come out slightly tapered, wider at the top than the bottom, which matters for a snug fit through the full thickness. Third, machine reality: backlash (lost motion when an axis reverses), tool deflection under load, thermal growth, and a slightly dull tool all nudge the result by a few hundredths to a few tenths.

Worked example: model a 10.00 mm slot, cut it on a laser with a 0.2 mm kerf without compensation, and you may measure about 10.2 mm - loose for a 10 mm tab. Cut the same slot on a router with a 6 mm bit centred on the line and it opens to roughly 16 mm, wildly wrong. And crucially, these numbers drift: a dulling laser tube, a new sheet of denser ply, a warmer room, a fresh cutter - each shifts your kerf a little. That is why compensation is never a fixed constant you memorise once; it is a value you measure for this machine, this material, today. None of this is failure - it is the physics you design around by adjusting the file, not by blaming the machine.

Put it together and a real joint is designed, not hoped for. Decide the fit you want (does this tab need to slide, click or lock?), then size the mating features so that after kerf and spring-back the actual parts land in that relationship. For a friction-fit slot on a laser, that often means drawing the slot a few tenths under nominal so the burnt kerf opens it up to grip the tab; for a clearance hole, drawing it a few tenths over. A couple of design touches make fits far more forgiving: a small chamfer or lead-in on the leading edge of a tab guides it into the slot square instead of wedging on a corner, and on brittle materials a slight clearance plus a dab of adhesive is more reliable than a hard press that may crack. Think also about accumulated tolerance - a joint that is a tenth tight is nothing, but the same tenth repeated across a dozen stacked parts becomes a millimetre the assembly cannot absorb, so spread adjustment across a run rather than fighting it at the last joint.

But you do not guess the number - you test cut. The single most useful thing a maker makes is a kerf/fit gauge: a small offcut with a row of slots stepped in 0.1 mm increments, cut in the real material on the real machine at the real settings, then offered up to the mating part to find which slot gives the fit you want. That measured offset becomes your compensation for every joint in the project. It takes five minutes and one scrap and saves a whole sheet of guesswork. This is the maker's discipline in one habit: never cut the final part until a test cut has told you what your machine actually does to that material today. Machines, materials and blades drift; the test cut is how you catch the drift before it costs you a full sheet and an afternoon.