Engineering Stack Exchange is a question and answer site for professionals and students of engineering. It only takes a minute to sign up.
Sign up to join this community
I can not really understand how people decide what tolerances to set for a part or assembly. For example:
When can I choose 0.2 mm and when 0.002 mm; and if I choose 0.002, why didn't I choose 0.001 or 0.004 or any other number?
Is there a Handbook, a standard, or is it mostly about experimenting and experience?"
I think you need to understand what a "tolerance" means in an assembly items. My token view is, a tolerance is the permissible deviation of a part from its ideal design dimension. Additionally, under the non-ideal situation, the assembly will not lose its intended functionality, and desired level of performance. After that, you may start to tighten the deviation, which will be based on the economic, and feasibility considerations as described by NMech. So the specification of a tolerance is not done at random, but is the result a calculated/weighted decision.
Hope this helps.
This is a very difficult answer to answer within a single post but I'll give it a try.
The very first thing you need to remember is that tolerances are indirectly related to cost. More precisely, having tight tolerances means that two objects will be more closely matched compared to two others with looser tolerances. However in order to achieve tighter tolerances, you need to use better machines, different processes and/or better trained personnel.
In the following graph you can see a comparison of the relative cost( in log scale), with respect to a few different processes. Also you can see for the different processes typical tolerance capabilities for the process.
Obviously, having tighter tolerances is equivalent to dimensional accuracy. The dimensional accuracy is desired because having a tighter dimensional envelope results in more predictable behavior of the product.
So bottom line is that you should strike the balance between manufacturing cost and the dimensional accuracy..
In general, ISO 286 determines the international tolerances grades for nominal sizes. The symbol for each grade is IT followed by an integer from 1 up to 20 (the only exception is IT01 which is tighter that IT1). The higher number IT grade the looser the tolerance. Also, above IT6, every 5 grades there is a tenfold increase.
In general, the following IT grades are used:
A commonly used system in the fitting of holes and shafts revolves around the concepts of
Under this system, hole dimensional tolerances are denoted with upper case Letters followed by a number (e.g G6, H7), while shaft dimensional tolerances are denoted with lower case (h7, p6).
Letters prior to H (e.g. ABC ) are related to bigger holes and, smaller diameters for shafts. Smaller numbers are related to tighter limits on the tolerances.
There are standards. But that's really putting the cart before the horse.
Imagine you're designing ..anything. By default the tolerance is whatever you can expect from the fabrication process if everything is done very poorly, and carelessly.
Is the part still acceptable? If so then you're done, no tolerance needed (practically speaking).
Most of the time that will not be the case. So you start saying things like "this slot must be at least 10.1 mm's wide, but not more than 10.5, or the part won't fit". That's all tolerancing is.
You're basically telling the fabricator how careful they need to be, and what kind of processes they can use. Do they need to machine it? or can they just cut it with a jigsaw? That kind of thing.
Tolerancing also depends somewhat on how much trust you have in the manufacture, the stakes, and how many lawyers are involved. For example, if I'm just having the local machine shop make a simple part for me, I know approximately what processes they will use to make the part and what kind of tolerance to expect. From there I'll specify only the tolerances where I know special steps will be required. If on the other hand I was going to have 10 thousand parts made on a contract, I might tolerance every single dimension.
3rd edition Marks HandBook circa 1923 is what I use. When the local library re-opens, check out the modern versions in the reference section.
ISO 2768 is a good pointer towards tolerances on lengths, angles and some geometric tolerance things. Engineers Edge have bits of it tabulated here. It's only valid for machined parts but it's a good start. There's an equivalent standard for welded parts, castings and presumably polymers.
Generally aim for 'medium', I'm yet to find a machine shop that doesn't work to that level by default, often choosing 'coarse' wont save you any money because shops will hit medium without trying anyway. You can either declare the standard on a drawing and invoke all of it (read the standard first though, clause A.4 causes some controversy), pick the numbers out and put them in a block tolerance, or just use them in your dimensions.
Additionally EE have a tabulated list and guide on preferred hold/shaft sizes here, which is taken from ISO 286.
