Tolerance analysis ISO2768 5

[KENAT]

I’m in the US working to ASME standards. I used to work in the UK where we invoked our British Standard version of the ISO standards.

A few weeks ago I had to check a print of a new part which was a minor change from an existing part.

One main component it interfaces with is German and on the drawing references ISO2768 FEIN (fine, in case you didn’t guess) I don’t recall ever working with this tolerance standard in the UK. I found extracts that I thought gave me what I needed on the web.

I did some tolerance studies of the interfaces and came up with big clashes at worst case.

I went back to the designer and he said that while he couldn’t argue with the numbers the old version worked etc. He contacted the vendor to verify my interpretation of the standard.

I have an email now from the vendor basically saying my interpretation is completely wrong, trouble is I don’t have ISO2768 to be sure and the way the email is worded either A. the person writing it doesn’t really know what they’re on about or B. their English just isn’t fantastic.

For instance I have part of a hole pattern, two threaded holes in line. The first is 36.66mm from the 0 ordinate. The second is 103.34mm from the 0 ordinate. Nominal spacing therefore is 66.68mm. From the extract of the ISO I found both 103.44 & 36.66 are +-.15mm. Therefore I assumed that the spacing is 66.68 +- .3 (.012”) which I was using in hole position calculations as pos dia .033”.

The vendor is saying the +-.15 applies not only to the holes relative to the 0 ordinate but also their spacing to each other. So if one moves away to be maximum distance from 0, the other at least has to be on nominal or further away from 0 etc.

Does anyone know if the vendor is right, or can point to a website where this is explained? (I need to give the designer an answer in the next few days and am not sure I can justify buying the standard or get it in time.)

Further does this ISO say anything about assumed coaxiality or position tolerance of circular features (holes)?

It’s bad enough trying to work out the drawing given it’s 1st angle projection and my brains stuck in 3rd, the addition of this tolerance is just icing on the cake;-).

Thanks for any assistance.


KENAT, probably the least qualified checker you'll ever meet...

 

[KENAT]

Having looked at it I should clarify that the drawing only says fein, doesn't ref a letter grade which I believe is needed to invoke part 2 for geometric tols, please correct me if I'm wrong.

Neither of the below gives me the answer.

thread182-93945

thread182-170720



KENAT, probably the least qualified checker you'll ever meet...

 

[powerhound]

I haven't worked much with ISO standards but I have worked with IT tolerance grades which may be similar to what you're looking at (maybe not), but either way, in all my time working in machine shops, the only thing that any tolerance was applied to was the exact dimension, not an extrapolated association between features that didn't have a dimension between them. My opinion is that the tolerance only applies to each dimension from 0 and not to the difference between the 2 features. In your case, the first hole could be 36.66 -0.15 and the next hole could be 103.34 +0.15. While this will produce a centerline difference of 0.3 from the nominal difference between the two, you can't extrapolate a dimension between the two holes and give it a tolerance of +/-0.3. If you nail the 36.66 dimension perfectly and then put the next hole at 103.04, it will be in tolerance with your extrapolated dimension of 66.8 +/-0.3 but it will be out of tolerance with the print dimension of 103.34 +/-0.15.
My opinion is that both you and your vendor are incorrect. I've stated in the above paragraph why I felt that your line of thinking wasn't exactly right but if your vendor thinks that one hole should follow the other when the dimensions of the holes are originating from another point, independent of each other, he's incorrect as well.

Powerhound
Production Supervisor
Inventor 2008
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[KENAT]

powerhound, you have a point I was being a dumb*** when I wrote that, thanks.

The 'equivalent position' tol should be based on the +-.15, not sure what I was smoking at that point;-) In fact that's the value I used in my calculations not .3.

However my point on the hole spacing effectively being 66.68 +- .3 on centerline is correct even from what you say. This is what the Vendor is arguing, he's saying that it's 66.68+-.15.

Either the ISO says something about this or he's smoking something even better than I was when I put my first post.

I just want to get a feel for which. The designer I'm working with isn't the most cooperative at times so I want to try and make sure I'm right.

KENAT, probably the least qualified checker you'll ever meet...

 

[powerhound]

KENAT,
I absolutely agree that the tolerance is effectively +/-0.3 between the holes but what I was saying is that it won't work if you're trying to achieve the center distance between the holes as well as the dimension from the edge of the part (or whatever feature the holes are called out from).
I can't imagine in my wildest dreams that the ISO standard says something along the lines of ignoring a hard callout and somehow relating the position of one feature to another even though they aren't called out relative to each other. The way to relate the position of one hole to the other is to show a dimension between them, it's as simple as that. My new and improved opinion is that either (a) your vendor knows something that we don't or, (b) he's still wrong.


Powerhound
Production Supervisor
Inventor 2008
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[KENAT]

Thanks powerhound. I just got another two of our German Interns to take a look and they too think that you end up with +-.3 between the holes if dimensioned this way. One's off to ask a couple of others their opinion.



KENAT, probably the least qualified checker you'll ever meet...

 

[KENAT]

OK, I now have 4 German interns who agree.

Does your opinion, 4 interns & mine outweigh one Vendors Engineer?

Ken

KENAT, probably the least qualified checker you'll ever meet...

 

[JMarv]

Kenat,

The copy I have of ISO 2768-1 (1989) doesn't make any specific mention of assumed coaxiality or positional control. It's just a general tolerance for untoleranced dimensions. I don't believe it's meant to take the place of properly added positional control. (The spec does specifically state that is doesn't apply to basic dimensions). I believe your interpretation is correct.



Joe
SW Office 2006 SP5.1
P4 3.0Ghz 1GB
ATI FireGL X1

 

[KENAT]

Thanks JMarv.

I appreciate you looking, it confirms what the excerpts I've found on the Web and what the interns tell me the german version of machineries hand book says.

The more I think about it the more I'm convinced what the Vendor is saying isn't true. I think it may be the language barrier but at the same time I meet so many people that don't seem to have a clue about tolerances that I'm loathed to make that assumption.

Now I just have to work out a way to break it to the Designer. I think that can wait till after the holiday (labour day for non US types).

KENAT, probably the least qualified checker you'll ever meet...

 

[powerhound]

Maybe you can get your vendor to explain his rationale for why he thinks the way he does about this issue. I'll be willing to bet that's it's nothing more than a notion he's had for years and has just never been challenged about it. On the other hand if he whips out the ISO standard and shows that he's correct, we'll all be eating crow for awhile.



Powerhound
Production Supervisor
Inventor 2008
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[KENAT]

If I had more time, I would but I'm out in few minutes and the designer needs an answer when I get back. Plus like I say I think there are communication issues so it would probably be painful.

Plus I'm pretty sure this would just add fuel to the fire of this particular designer complaining about having his drawings checked, why are we invoking military standards etc. (you've seen my other posts).

Thanks,

KENAT, probably the least qualified checker you'll ever meet...

 

[ajack1]

KENAT I would say you are absolutely correct, to the best of my knowledge (but I am sure others know more) no ISO standard works on calculated dimensions only actual ones.

Unless I am missing something simply replacing the 103.44 dimension with a 66.68 would do the trick in the example you give, however this only works for two dimensions in a chain. The easiest (not best necessarily) solution for the designer would be to change the +/- 0.15 to +/-0.07 and I would guess this would be the option they may take. This may of course make the part more expensive to produce.

I can see your problem is to ensure the prints are to standard and nothing else, has this always been the case at the company? Most machinists prefer ordinate dimensions rather than having to add A to B subtract C and then add D for obvious reasons, this again may be done to save costs. If the parts is produced on a CNC for example neither way will matter, if not it could do, so the designer could be following what he has been told to do in the past.

As I see it you are absolutely correct but are in danger of increasing the cost part, but that is probably not your concern.

 

[joebk]

I work for a company headquartered in Germany, they invoke ISO 2768 on all drawings. I have version dated 1989-11-15. Man is this standard a pain in the butt.

There are two sections of the standard, 2768-1 deals with "tolerances for linear and angular dimensions without individual tolerance indications". 2768-2 covers "geometrical tolerances for features without individual tolerance indications".

The way the standard is invoked on the drawing doesn't follow the guidelines in the standard so I am not sure which sections apply. For reference, the German title block at our company indicates "ISO 2768-mK". "m" indicates which tolerance grade applies from 2768-1 and K indicates what tolerance grade applies from 2768-2. Sometimes on our drawings it is specified as "ISO-mK-E" indicating that the envelope principle applies.

Given the spec you describe, I would guess that only section 1 applies because a tolerance grade from section 2 is not included. But this is a bit of a guess on my part. 2768-1 only applies to dimensions on a drawing that do not have a related tolerance specification. So it cannot be applied to calculated values.

2768-2 applies geometric controls that are otherwise not specified (runout, parallelism, symmetry, circularity, cylindricity, straightness, and flatness). There is a note in this section in regards to coaxiality of holes.

IMO here is the kicker with these standards. At the end of both standards there is a note that states "Unless otherwise stated, workpieces exceeding the general [geometric] tolerances shall not lead to automatic rejection provided that the ability of the workpiece to function is not impaired." What a load of nonsense! It is like putting a tolerance table in the title block and a note saying that the tolerances apply only if there isn't a problem in the application! Bah! This causes big problems when we try to source European designs here in the USA.

 

[KENAT]

Ajack, the drawing invoking the ISO isn't ours, it's a vendors. I'm just trying to make sure our mating components will work with it. I can't make the vendor change their drawing to have 66.68 instead of coming off the 0 'datum'.

I'm not a fan of ordinates but don't normally make people change them, also I usually dimension from a datum, which effectively gives the same as ordinate dimensioning in most cases. Either way the drawing isn't primarily there to make life easy for the machinist but this is a different philisophical argument for another time & place.

My job is not just to ensure prints are to a standard, I'm not quite sure what I posted to give you this impression.

My job is to make sure the drawings are accurate, have all relevant detail, can be taken to any competant vendor, verify Form Fit Function (when time & available info permit), generally free of mistakes etc. Enforcing the standard is just a means to an end to help achieve many of those goals.

Anyway, gotta go.

joebk, thanks for the info.

KENAT, probably the least qualified checker you'll ever meet...

 

[KENAT]

I just got a copy of the standard and looked through and as a couple of you say it says nothing about the same tolerance also applying to 'calculated' dimensions and there being no compounding of tolerance.

It does reference ISO 8015:1985 Technical drawings - Fundamental tolerancing principle. I'm pretty sure I would have looked at this back in the UK (I used to consult BS8888 regularly) and I don't ever recal there being anything implying that tolerances don't stack up.

All my tolerance calculations there, some of which were verfied buy others, assumed tolerance stack up.

joebk, I just read the last section A.4. where it talks about "Unless otherwise stated, workpieces exceeding the general [geometric] tolerances shall not lead to automatic rejection provided that the ability of the workpiece to function is not impaired." and was as bemused as you.

I thought the point of tolerance on a drawing was to define what was acceptable. Not give a vague suggestion of what you'd like but that more may be acceptable.

In fact I think I have an issue with this standard overall, it seems more concerned about suiting manufacturing than ensuring functionality! Sure manufacturability is very important, but not at the expense of function!

KENAT, probably the least qualified checker you'll ever meet...