Metric tolerances in title block 4

[JJAV1983]

Hi,

I recently started working for a new company, I noticed that the default metric title block we are using only has the specifie tolerance as follows:

TOLERANCE +/- 0.1 (mm)

All current and past drawings are dimensioned with 2 decimal places. So for example right now if we dimensioned the width of a plate as 19.10 mm, with the only reference we have in title block (Tolerance +/- 0.1) this width could be made at 19.00 mm or 19.20 mm. But what would happened if the width is 1900.00 mm and we don't need a tolerance as tight as +/- 0.1.
There is no specification for decimal places whatsoever, the only thing it says is: TOLERANCE +/- 0.1
We design from PCBs to low, medium and line voltage lighting systems and every single aspect of the fixture (housings, electrical boxes, brackets, etc). I really think we need to make some modifications to the title block, as the specification is real vague.

I was thinking something like this:

UNLESS OTHERWISE SPECIFIED:
X +/- 0.5
X.X +/- 0.3
X.XX +/- 0.13

Thank you for your advice.

JJAV 1983

 

[MintJulep]

Are you ever likely to make a PCB that's 1900 mm in any dimension?

 

[JJAV1983]

Certainly no, I meant to say 190 mm, and that was for the box/housing that the PCB is going to installed on.

 

[juergenwt]

1983 go here:

http://www.ramo.se/iso_2768_english.htm

or here:

http://www.marylandmetrics.com/tech/DINISO1302extract.htm

 

[dgallup]

First you need to know (and tell us) what drawing standards you are are using.

Second, every metric drawing standard I am familiar with does not use the number of decimal places to indicate tolerance. As linked above there is an ISO standard that lets you pick a class of tolerances (fine, coarse, etc.) and the default tolerance varies with the nominal size.

Third, many companies (including where I work) use a single default tolerance for a drawing. This can change from drawing to drawing so you can set an appropriate value.

Forth, you can always put an appropriate tolerance on each and every dimension. I encourage this because it involves consciously thinking about the importance of each dimension and the impact of the tolerance.

----------------------------------------

The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.

 

[drawoh]

dgallup,

I agree strongly with your point four.

Thinking about each and every dimension is worthwhile. Also, it does not take long to apply tolerances to each and every dimension, unless you realize that the tolerance does not work. Now, you have some re-engineering to do to make sure everything works.

--
JHG

 

[JJAV1983]

dgallup

1. ISO standard.

2.Should I just refer to ISO standard in title block, i.e :
UNLESS OTHERWISE SPECIFIED TOLERANCE: ISO 2768m

3. What do you use as a single default tolerance?. In your third statement ("This can change from drawing to drawing so you can set an appropriate value") did you want to say: This can change from drawing to drawing so you CANNOT set an appropriate value.

4. I totally agree with you on this. We should apply appropriate tolerances on every dimension, although sometimes your drawing can get really messy, using a sheet size A4 don't help also. That's why I wanted to know default tolerances on metric drawings so we can apply this to our format.

 

[looslib]

The official designation of ISO 2768 callout consists of 2 letters.
2768-1 specifies linear and angular dimensions and has 4 letters (f,m,c,v) that specify class.
2768-2 specifies feature tolerances and has 3 letters (H,K,L) that specify class.
When applied to a drawing, you need both; ISO 2768-mK would be a valid callout. Note there is a dash between 2768 and the clasees.

As for a default tolerance, it is not needed when using ISO 2768 as your standard since the standard determines the tolerance based on the size of your part.

Also, note that metric dimensions do NOT use trailing zeros. So your original note the size should be 19.1 with a range of 19 to 19.2, if you use a 0.1 tolerance.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[CheckerHater]

When applied to a drawing, you need both; ISO 2768-mK would be a valid callout.

 

[pmarc]

JJAV1983,
Are machined or sheet metal parts amongst products offered by your new company?

 

[JJAV1983]

pmarc

Yes we have machined and sheet metal parts our line of products.

 

[pmarc]

I see you have PCBs. Plastic parts too?

 

[JJAV1983]

No plastics parts at all.

 

[dgallup]

3. What do you use as a single default tolerance?. In your third statement ("This can change from drawing to drawing so you can set an appropriate value") did you want to say: This can change from drawing to drawing so you CANNOT set an appropriate value.

No, I meant what I said. If I have a precision machined small part I might choose a +/-0.1 mm default tolerance. If I have a vacuum formed plastic tray to hold my parts I might choose a +/-1 mm default tolerance. In our CAD system the default tolerance is read from the model, our part template has the default tolerance set to +/-0.2 mm but I can change it and the drawing will show that.

There is nothing worse than having excessively small default tolerances and a drawing with all nominal dimensions. It tells me the "designer" gave absolutely no thought to tolerances and how the part functions.

----------------------------------------

The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.

 

[pmarc]

OK, thanks.

I asked because ISO 2768 is intended for: "[...] dimensions of parts that are produced by metal removal or parts that are formed from sheet metal" and it "[...] may be suitable for use with materials other than metal" and for "[...] features manufactured by other processes", but with special examination required.

Regardless whether you decide to switch your general tolerances to ISO 2768 (poor choice, in my opinion) or not, I thought I should clearly mention this.

 

[CheckerHater]

So, there are enough negative choices for now:

[ul]
[li]You can use number of decimals NOT, because metric dimensions cannot have trailing zeros both in ASME and ISO.[/li]
[li]You can use one single default tolerance NOT because your parts span over wide variety of sizes.[/li]
[li]You can invoke international standard ISO 2768.[/li]
[li]You can invoke American standard ANSI B4.3.[/li]
[/ul]

What are the positive choices left?

[ul]
[li]You still can use International Tolerances per ANSI B4.2, creating note like: “UNTOLERANCED DIMENSIONS HOLES H12, SHAFTS h12, OTHER +/-IT12/2”[/li]
[li]You can actually create a table based on ISO 2768, or ANSI B4.3 and place it in or near your titleblock:[/li]
[/ul]

 

[dgallup]

CheckerHater

I do not understand why you say:

[ul]
[li]You can use one single default tolerance NOT because your parts span over wide variety of sizes.[/li]
[/ul]

The single default tolerance DOES NOT HAVE TO BE THE SAME ON EVERY DRAWING. You just set a reasonable default tolerance for the part on each drawing. What is so difficult about this? Just like ISO 2768 lets you choose a class appropriate fro your part.

----------------------------------------

The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.

 

[CheckerHater]

Ok, let me be more specific.

I’ve got impression that OP found the technique unsatisfactory, because one could encounter features of different size within the same part; so he was looking for possible alternatives.

Naturally, you can use different tolerance values for different parts, but you still have to cover features that are too big or too small, for example use direct tolerancing on them.

And, yes, there’s nothing wrong about 2768, it just appears to be unpopular.
This is why I suggested ways of creating your own “class” by other means.

 

[DiegoLGraves]

I have to say I like 2768 because of the note to not automatically reject parts because they don't meet the tolerance. If they fit, use them. We got a big kick out of this note when we first started making parts to this standard. The inspector brought the parts to engineering and we'd say give me a minute, part fits ok, stamp it accepted. Provided a class of entertainment. That said we are most often fabricating to the tolerance rather than designing based on it.

Regards, Diego

 

[JJAV1983]

Thank you for the advice,

I think that CheckerHater suggestion will be the best option. I am just thinking if it would be valid to say:

UNLESS OTHERWISE SPECIFIED:
TOLERANCES: ANSI/ASME B4.3 (in case of using American Standard)

dgallup

When you said: "... single default tolerance DOES NOT HAVE TO BE THE SAME ON EVERY DRAWING. You just set a reasonable default tolerance for the part on each drawing..." You meant for each different size drawing (small part/big part) I would have to go and change the default tolerance?...

As you said it might not be a big deal, I am just thinking maybe one day a designer will forget to adjust that part in the title block and the end result will not suit the design intention. Just trying to avoid that type of problems in the future.

Thanks.