2
$\begingroup$

I have part that I'm dimensioning and setting tolerances on. Some of the dimensions/features have engineering requirements (e.g. press fit) and I have the tolerances set correctly (e.g. H7).

But I have some dimensions / features don't have any engineering requirements. They are usually outside dimensions or "free" surfaces that don't interact with any other parts. Technically the tolerance could be +100% of the nominal value. But this just seems "sloppy". I would like the parts to be roughly uniform. So how can I communicate on my drawings that the dimension is not critical without supplying an outrageous tolerance? Is there a rule of thumb for this sort of thing? Say 10% of nominal dimension?

Improve this question
$\endgroup$
2
  • $\begingroup$ It depends on the material and manufacturing process. You don't want to put on a tolerance that will make the part more expensive by requiring extra checks or slower processes. $\endgroup$
    – Jonathan R Swift
    Jun 26, 2020 at 1:09
  • $\begingroup$ A useful requirement I have heard of was "as cast." That was put on a piece of cast steel for the dimensions that did not matter. Saved loads of money in not having to verify the dimensions that did not matter and no surface requirements either! $\endgroup$
    – Cort Ammon
    Jul 9, 2020 at 3:24

3 Answers 3

Reset to default
3
$\begingroup$

There are general tolerances, often defined for different industries. You cannot expect that a surgical instrument is designed with the same general tolerances as a drilling rig.

If you have found a norm for your industry, e.g. this ISO-standard, than there are still different classes of "tightness" you can choose from. Here should just check what is appropriate for your design such that it still fits/works. In my experience most companies have the general tolerances on their drawing templates by default.

Improve this answer
$\endgroup$
2
  • $\begingroup$ This is a good start you should expand a bit on this though, like telling its called a general tolerance and defined in what standard how to apply it etc, so its not a link only answer. Care should be taken though general tolerances may sometimes be tighter than you need. But then things arent manufactured by hand anymore $\endgroup$
    – joojaa
    Jun 26, 2020 at 5:56
  • $\begingroup$ Yes, blindly applying the general tolerance can add cost through requiring inspection. It also can make sense to eg. apply a surface deviation geometric tolerance instead of these linear values such that the error is agnostic of scale - works well for CNC and 3D print etc. $\endgroup$
    – Jonathan R Swift
    Jun 26, 2020 at 8:52
2
$\begingroup$

If you use ASME Y14.5, typical implied tolerances are +/-:

1/64 for fractional dimensions

0.01 for dimensions to 2 decimal places

0.005 for dimensions to 3 decimal places

0.0005 for dimensions to 4 decimal places

You just list all these and whatever other common requirements you have in your drawing block for the part. This way every feature is inherently dimensioned. Generally +/- 0.010" is easily achievable for machined parts.

Improve this answer
$\endgroup$
2
  • $\begingroup$ I'm curious then how you pick a decimal place for dimensions? I'm reproducing an existing part that I can mic down to 4 decimals. But that seems overkill. $\endgroup$
    – tir38
    Jul 9, 2020 at 2:08
  • $\begingroup$ Depends on the form, fit and function for each dimension. If it's a feature that is a tight fit with another part it's usually tolerances to .001". If it's just the overall form of something that doesn't matter .1" is fine. $\endgroup$
    – jko
    Jul 10, 2020 at 12:24
0
$\begingroup$

Bound the problem from two different directions.

First, start with your process capability. What tolerance can you actually hold? This will vary greatly depending on whether you are doing casting vs milling vs grinding etc. If you have a bunch of similar parts lying around, measure them and compute the standard deviation. Remember that 68% of parts will be within +/- 1 std dev, 95% within two, etc. E.g. if you have a mill that's producing parts with a standard deviation of say 0.010", then only a few per million would be outside of +/- 0.060". That sets your lower bound. Any less than this, and you'll be scrapping parts that you don't want to scrap. If you don't have any similar parts, then do some research on typical tolerances using your process, whatever it is, and probably round up a little.

Then, thing about what dimension you need the part to have to satisfy fit form and function. You said it doesn't have any engineering requirements, but it does have to have something. If the nominal dimension is 2", I'm sure the part wouldn't work if the shop gave you something that was 200". Figure out the biggest and smallest parts that would actually work. This sets the upper bound of your tolerance. E.g. maybe it's +/- 1".

So now you've got a range. in our example above, if your tolerances are any tighter than +/- 0.06", your shop can't make them and that will make it expensive. If it's looser than +/- 1.00", the parts won't work. Anywhere in between will be perfectly fine, so just pick something that range. Split the difference and call it +/- 0.5" and you're done.

Improve this answer
$\endgroup$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge that you have read and understand our privacy policy and code of conduct.

Not the answer you're looking for? Browse other questions tagged or ask your own question.