I'm currently generating a set of pads for a footprint found in a datasheet. All of the length values in the footprint have min/max values e.g. 1.8 +- 0.1 Should I be using the 'middle' value, and if so, why do manufacturers bother with the min/max values?
Of course you have to pay attention to min and max values! This should be self-evident. Every manufacturing process has variations. There is no such thing as a fixed exact dimension. With the min/max values, the manufacturer is telling you what range the parts you will receive will fall within. You could get a whole batch right at one end or the other of that range. If you want your board to be reliably produced, it has to work properly with parts anywhere within that range. This should be obvious.
For example, if some surface mount chip is specified with a nominal .3" distance between the ends of the pins with a 10 mil tolerance, what exactly does the .3" spec mean? Nothing. It's only there to give you a quick conceptual idea of the size, but otherwise they are saying the size falls from .290 to .310 inch. Let's say you center the chip at the origin when defining the package in your CAD system. That means the absolute coordinate of the ends of the pins will be half the width. The ends could extend as far as .310"/2 = .155" from center. Of course there will always be some placement error and you want the pad to extend a little past the end of the pin for a good solder miniscus and possibly to ease manual soldering in case you ever need to. My general rule of thumb is to add 20 mils for all the above. That's a general rule. There are reasons you might want a bit more or less depending on how the chip will be placed and soldered and some details of the process. In this example, we'll go with the general 20 mil rule. That means the ends of the SMD pads need to be at the absolute coordinate .175".
The same logic applies to the inner edge of the pad. Again you look in the datasheet and find the minimum distance from the center of the chip where the pin can come down and touch the board. On the inside, you don't need 20 mil of additional length. I usually add about 10 mil, although particular processes may dictate something different.
Using this logic, you end up with a footprint that will nicely accept any chip the manufacturer sends you. If it's a standard footprint you may only want to enter it into your CAD system once (at least for the general case). There may be slight spec differences between manufacturers. It is a good idea to check datasheets from a few different manufacturers for the same supposedly standard footprint. This gives you a better idea of the true variation out there. Usually they are close, but there can be small differences.
It may be a bit confusing that there's a difference between who's job it is to guarantee that the manufactured sizes are within spec:
The component manufacturer has to make sure that the actual part complies to the package drawing and lies within the tolerances.
You, being the one who is responsible for the PCB, are the one who has to make sure that the actual, real PCB is within the specification of the recommended solder pad layout. The tolerances are there to help you: As with anything real, you won't be able to manufacture a board with 1.8 mm and +/- zero tolerance, but you can make a board with 1.8 +/- 0.1 mm.
What the datasheet tells you is that any part within worst case tolerances will be good on any real board within worst case tolerances. If they just gave you nominal values, you would be facing the impossible task of making a real board with theoretical, ideal tolerances. Thus, again, the tolerances are there to help you, they're not created to have you worry: Specify the nominal (typ.) values when creating your decals, and relax in the comfort of +/- 0.1 mm when having the actual board made.
Sometimes, you will find different drawings between various manufacturers for a part that's practically derived from the same standard case outline. If you wish to have decals that are good for parts sourced from multiple companies, you can attack this problem from two sides:
Start with the available drawings and specifications: It helps a great deal to compare similar drawings from a number of different manufacturers; say, for example, 0805 capacitors from AVX, murata, Kemet and whatnot, or MSOP-8 ICs from TI, Fairchild, Linear and whoever. Then, try to create footprints that agree with any of these manufacturers' standards and min/max tolerances. If you have access to sources that are not specific to one single manufacturer, like IPC (Association Connecting Electronics Industries) or JEDEC, and you can bring them to agree with what you've figured out, even better.
Start with information based on practical experience: Ask your place-and-solder shop what works best for their soldering processes (reflow?, wave?) and machines (temperature profile?, type of solder?). They will likely know that pads with a slightly larger or smaller dimension in one or another orientation help them to avoid unwanted things like tombstoning of chip capacitors or resistors.
Ideally, all the information you can gather will not contradict and you end up having Your Pefect DecalsTM.
Related, but not a duplicate: The "right" 0805 footprint land pattern