Hi,
these matters are normated: you should look at what it is specified in the Norm you want to apply.
The tolerance are divided in "classes" depending on the dimension range, but the division in classes can slightly vary between a Norm and another...
Do you use ISO2768 for your standard tolerancing? I think this is what cbrn was referring to, they have class f, m, c, v relating to (for your length) ±0.5, ±1.2, ±3, ±6 mm as normalized tolerance for "length" dimensions.
If you are asking what is possible, much depends on the machinery...milling machine like Bridgeport or new 0.1 micron CNC controlled machine has different capability. In my experience you might be able to hold ~0.5mm (±0.25mm) with good machine in temperature controlled environment...
You may want to find out how much the accuracy costs. There is often a steep price increase at some point that you may be able to avoid with a slight design change.
The concept of "standard tolerance" is just wrong. How can a standards writing body possibly have any idea what tolerance is required for your specific design?
Tolerance is a design function. The designer of a part, assembly or system must make the determination of what manufacturing variation can be tolerated.
Those who participated in writing the standard did account for manufacturing variation to determine the production method, this is why they have four classes (partial list):
>0.5 to 3 >3 to 6 >6 to 30 >30 to 120 >120 to 400
f ±0.05 ±0.05 ±0.1 ±0.15 ±0.2
m ±0.1 ±0.1 ±0.2 ±0.3 ±0.5
c ±0.15 ±0.2 ±0.5 ±0.8 ±1.2
v ±0.5 ±1 ±1.5 ±2.5 ±4
Was probably very good when all used manual machines and journeyman operators, now we do much better than this. Same like industry extrusion standards or cast association standards.
I thank you all for your comments, my question originated from the fact that a common cnc machine is accurate to give a true position of 0.004 mm, if so, what are the main reasons that class f tolerance gives +\- 0.05, and what measures should be taken to achieve cnc machine tolerance of 0.004 ?
Hi,
I don't want to be polemic, but MintJulep probably did not think about the fact that not all the dimensions in a part do are functionally important; if you tolerate just ALL the dimensions which you have in a complex part, you will make it impossible to interprete and thus to make; or, it may be that for your part the ISO classes are too coarse, but then it's a matter of YOUR design, not of the ISO !!! Where I work we design parts that can be very complex: some of the dimensions are tolerated, other fall under the generic guideline "dimension tolerances where not otherwise specified: ..." and of course this is done in tabular form; just a last thing: if you tolerate everything, you DO HAVE to make sure that everything is coherent, i.e. you have to make a very extensive analysis of the dimensional chains!!!
To return to Asherktz's question: if you have a milling machine that is able to respect micron-class deviations, that's good and if you really need it for the design, then feel free to use it; but I wouldn't push the machine to its limit: 0.004 mm deviations over a 1000 mm length are possible only with an extremely accurate setup, extremely accurate calibration, extremely accurate thermal stabilization, and so on; all these things will COST a lot!!! If this machine is 0.004 mm capable, then most probably it will be able to handle 0.01 very easily, I mean with short stabilization etc. Just an example taken from my experience: in my previous work we manufactured high-precision shank-mills in tungsten carbide; we measured that, when we were manufacturing a dia.6, 90 mm long mill with 32 mm cutting length, we had 6 micron deviation on the cutting-edge width just when the protection door of the machine was exposed to sunlight or not; the machine (a Rollomatic 600, a real jewel) took 40-50 mn to thermically stabilize by executing idle cycles...
ALL dimensions must have a tolerance. If you have no tolerance you are in fact stating that your design cannot tolerate ANY deviation from from the nominal or basic dimension called out.
If you are making a design decision that a title block default, or an ISO standard list of tolerances is appropriate for your design, fine. If you just blindly accept a set of "standard tolerances" you are not doing your job.
While our drawings have a standard tolerance for each quantity of digits to the right of the decimal (one/two/three places), it is definitely part of my job to consider the appropriate tolerance for each and every dimension. If the drawing standard tolerance meets all the requirements (manufacturability, cost, assembly mating, load path integrity, to name a few), fine. But I am responsible to actively make that decision for every dimension. And I believe the same is true for every engineer.
While I vaguely agree with all the philosophy being thrown around, out here in the real world I'm thinking about a 2 thou positional tolerance in 5 feet. (ie .05mm in 1600 mm).
That's two cigarette papers in a man's height.
Unless you are working on optical systems, or measurment systems, that does not seem like an unreasonable number. I routinly work with 3 sigma errors of 3 mm in that distance.
Cheers
Greg Locock
Please see FAQ731-376 for tips on how to make the best use of Eng-Tips.
Hi,
MintJulep & others: there might be a little misunderstanding... I'll try to clarify my position:
- tolerances are needed everywhere, because "pure-exact" dimension don't exist in reality
- not all the dimensions have to be explicitely tolerated in the drafting; a drawing will be interpreted like that: when the tolerance is not indicated, then the standard one applies; where purely indicative dimensions are specified, they must be identified as such ("control dimension" for example).
Nevertheless, it is possible to find designs where all the dimensions can respect functionality with the standard tolerances, so in these cases there is no need to be redundant.
In addition, I agree that a designer must know the what and why of every dimension he places, but, honestly, how many of you use a tolerance-analysis program or perform manually the whole dimansional-chains analysis by taking into account every possible interaction between dimensions? Honestly again, do everyone of you never accept some degree of "uncertainty" by enlarging the tolerance field where POSSIBLE (and please note that even this decision must be thought of, it's not an obvious one)? None of you ever saw contradictory tolerance indications? Isn't that an example of cases where the designer thought to do "better" and ended by doing "worse"?
Well, we are getting farther and farther from the O.P.'s question, I fear.
Everyone of us except Greg Locock missed that point: in which field will this 1600mm dimension be used?
And moreover, will the manufacturer be able to respect the tolerance with the adequate "stability" (i.e., which will be the dispersion? 1, 2, 3 or 6-sigma?)?
A last addition to the milling machines' capabilities: it's not because they use a 0.0001mm-precision optical measuring method that they will be able to respect a 0.1 micron tolerance!!! As Sreid said, only the sun entering through a window is able to send this precision directly into the wastebasket!
"I thank you all for your comments, my question originated from the fact that a common cnc machine is accurate to give a true position of 0.004 mm, if so, what are the main reasons that class f tolerance gives +\- 0.05, and what measures should be taken to achieve cnc machine tolerance of 0.004 ?"
A true position of 0,004 mm may, or may not be true for the MACHINE. However, there is usually a world of difference between the basic machine positioning tolerance and what is achieved in a machined part. One would have to go to extraordinary lengths to achieve a true position of 0,004 mm for a series of holes in a machined part. However, as stated by others in this forum, all it takes is time and money, both of which, in most organizations are in short supply. You should concentrate on giving the WIDEST positioning tolerance you can live with. Also, you should understand that standard twist drills are only capable of removing material, they are very unpredictable regarding true position. Precision boring bars solidly located in a precision spindle will get you closer to to a true position than any drill will, and will be quite consistent.
I would respectfully advise you not to try to design parts based upon the claims of machine manufacturers. They are usually extremely optimistic about the capabilities of their products.
In a past job I fought a tolerancing problem. Long and expensive story, but in the end it ended up being a problem with very small part movement within the fixturing.
I'm not sure if this is relevant to your cause but it is something which adds to the problems of holding a tolerance.
