Before we get into nozzle sizes and snap fits, let's start with the bigger picture. We need to use common language for defining the parts.
- Allowance is a planned difference between a nominal or reference value and an exact value.
- Clearance is an allowance defining the intentional space between two parts.
- Interference is an allowance defining the intentional overlap between two parts.
- Tolerance is the amount of random deviation or variation permitted for a given dimension. How much error can the part tolerate and still function?
Let's use an example. We want a 5mm pin to go into a 5mm hole, and we want a loose fit between them.
We've said 5mm, but which 5mm is more important -- the 5mm hole or the 5mm pin? Let's say other people have 5mm pins they want to use with our hole. In this case the pin dimension is out of our control, and therefore is more important for interoperability.
The loose fit is calling for clearance. Let's specify 0.2mm so they're free to turn.
We could add the 0.2mm allowance to the hole, giving a 5.2mm hole with a 5.0mm pin; we could subtract the 0.2mm allowance from the pin, giving a 5.0mm hole with a 4.8mm pin; or split the difference in any way we want, such as a 5.1mm hole and a 4.9mm pin. Because we specified the pin is more important, we'll add the allowance to the hole.
Now that we have defined our part, let's define other terms important to helping us understand the manufacturing process:
- Accuracy is the maximum dimensional variation between parts. (Another word might be repeatability.) Note that a machine cannot produce parts with a tighter tolerance than its accuracy.
- Precision is the size of the steps a machine is capable of. Precision is often confused with accuracy, but they are not the same thing.
Now we need to understand our machine's accuracy. The printer could print the pin larger than 5mm or smaller than 5mm. Or it could print the hole larger than 5mm or smaller than 5mm. To determine the printer's accuracy, we'll need to print some 5mm pins and 5mm holes and measure the differences between what we defined and what we printed. The difference between the largest and smallest measurements is our machine's accuracy. Be sure to measure the accuracy in the X, Y, and Z dimensions; a printer might have a difference between the X and Y axes that would affect the roundness of the parts. (If it's off, this can usually be adjusted in the machine's firmware through a calibration process.) Furthermore, we should test round parts, round holes, square parts, and square holes, as each printer can be different in how repeatable those parts are.
Let's say that the printer's measured accuracy for both round holes and round pins is +/- 0.2mm.
Then, we move to clearance. What is the minimum gap between parts and still do the job, and what is the maximum acceptable gap? As the designer, it's up to you to decide. In this example we said we want a loose fit, so let's define a clearance of at least 0.2mm between the pin and hole; but no more than 1.0mm or the parts will fall out.
Since the machine's accuracy is +/-0.2mm, the pin will be anywhere between 5.2mm and 4.8mm. The hole must therefore be 5.2mm plus clearance plus the accuracy of the hole. That gives the hole dimension as 5.6mm +/-0.2mm. The minimum tolerance condition would be an minimum sized hole (5.4mm) and a maximum sized pin (5.2mm), giving a 0.2mm clearance; the maximum tolerance would be a maximum sized hole (5.8mm) and a minimum sized pin (4.8mm) giving a 1.0mm clearance.
Note that a clearance of 1.0 mm is really sloppy. It might seem too loose for our application. We might think to tighten the tolerances to 0.05mm in order to reduce the clearance. But we've noted that a machine can't produce a tolerance tighter than its accuracy. If the printer can't produce a part that meets our specified tolerances, we would need to find a different way to manufacture or finish the parts.
In the metalworking world a common way to do this is specify the parts to be initially manufactured with intentionally maximal material. This lets us start with a smaller hole and use a bore or a drill bit to open it up to a more precise and round hole. We can do the same thing with a pin, by starting with a thicker rod and turning or grinding it down to make it more smooth and round.
In the FDM 3D printing world, we can do the same kind of thing at the workbench. First, print the parts with an extra wall layer (or two). The extra thickness gives more material to remove while drilling it out, or grinding it down, without weakening the part too badly. After printing, run a drill bit through the hole to clean it up. Or spin the pin in a drill motor's chuck and grind it down with a loop of sandpaper.
Of course any time you add a finishing operation, it's more labor intensive and therefore more expensive. So this isn't something we want to do on every part, but we can consider it.
Notice that when you define parts this way you aren't starting with the nozzle diameter or layer height. Instead, you're allowing the nozzle diameter, layer height, and the sum of all the causes of variations, to show up in the measured accuracy of the machine. Smaller nozzles, thinner layers, heated beds, or cooling fans may each contribute to improved accuracy, but it's best to factor in the cumulative impact of all the machine options.