Default Tolerances in Title Block 1

[phlyx]

We have a debate going on internally here as we attempt to re-design our title block for CAD. The debate centers around the default tolerance call-outs on inch unit mechanical drawings. Basically these are the defaults that are being debated :

- FRACTIONAL +/-
- 1 PLACE DECEIMAL X.X +/-
- 2 PLACE DECEIMAL X.XX +/-
- 3 PLACE DECEIMAL X.XXX +/-
- 4 PLACE DECEIMAL X.XXXX +/-
- ANGLES +/-

What numbers does anyone have for these values and is there any standard that covers this?

Thanks in advance!

~ Phlyx ~

 

[TVP]

ISO 2768 is one such standard that covers tolerances, but it is in SI units. I would assume there is a similar ANSI/ASME standard.

 

[arto]

ASME B4.1 covers cylindrical limits & Fits.

The old timers used to say half the smallest decimal place or fraction, i.e.:
for 1.23 it's +/-0.005
for 1.2 it's +/-0.05
for 1. it's +/-0.5

for 1-1/2", it's +/-1/4"
for 1-7/8", it's +/-1/16"

for 5/32", it's +/-1/64"

 

[haggis]

phlyx,

We (who?)use, and most drawings we receive from vendors are as follows:

Fraction - +/- 1/32"
One decimal place - +/- .010
Two decimal places - +/- .005
Three decimal places - +/- .002
Four decimal places - +/- .0005
Angles - +/- 0.5 deg.

In case of special circumstances you might want to "except as noted" to your block.

 

[TheTick]

Really, it depends on the process used to make parts. Any recommendations made without considering this are worthless.

"Great ideas need landing gear as well as wings."--C. D. Jackson

http://www.EsoxRepublic.com

 

[phlyx]

The process is machining of mechanical parts for O.E.M. machinery design. The notes in the title block are listed as UNLESS OTHERWISE NOTED so they only apply if no tolerance is specifically called out on a dimension. Just trying to get a feel for the industry standard. What we are close to settling on is :

FRACTION +/- 1/64
2 PLACE +/- .015
3 PLACE +/- .005
4 PLACE +/- .0005
ANGLULAR +/- 1/2-DEGREE

I assume these are varied in different work environments but must drive machine shops nuts if places have different values all over the place.

Good comments! Thanks!

~ Phlyx ~

 

[drawoh]

phlyx,

ASME Y14.5M-1994, the official dimensioning and tolerancing standard, allows you to control dimensions from a note. It says nothing about what the contents of the note ought to be. It does say that all dimensions must have tolerances.

How accurate do you need to be?

Don't forget metric.

JHG

 

[alexit]

I love SI units...our title block lists "ISO 2768" then "f", "m", or "k" depending upon the designated manufacturing processes...

 

[Mandrake22]

Here is our "boilerplate":
Fractional = +/- 1/32"
.XX = +/-.015"
.XXX = +/- .005
Angular = +/- .5°
We make agricultural equipment up to and exceeding 20,000 lb. Lots of fabrication and sheet metal. A fair amount of machining and casting. Wouldn't know what to do with a surface if I sat on one!

 

[automationbabe]

My last company left the tolerance block blank and the designer/drafter had to fill in the block according to their needs. The belief, which I find value in, is that you design a part with tolerances in mind, but set the tolerances to the design. If you are constrained by pre-determined tolerances, how effective is your design or your efficiency if you have to go retolerance the dimensions that don't match the preset block.

The varying tolerance block also made our vendor pay attention to what we were sending them and what they fabbed our parts to. At my current job, they have a set block, that is not set in stone, that I change the numbers on according to my needs. This through a few of our vendors off at first, but now they pay more attention and the quality of our parts are better IMO.

Regardless of industry, every part does not necessarily need the same tolerance and finish as every other part. Design and tolerance to form, fit & function.

Tick also made an excellant point. The process and specified finish can also have an impact. How many weldments do you see to the tolerances above? But a number of machinery designs use them.

Good luck with this one.

 

[MouseTrap]

I have to agree with Tick (again).......the tolerences for your company title block should depend on which process you are using. If you are cutting everything with a welding torch, it doesn't make sense to have tight tolerances that a milling or turning operation is capable of

You stated that your latest corporate 'general consensus' leaned towards the following..

FRACTION +/- 1/64
2 PLACE +/- .015
3 PLACE +/- .005
4 PLACE +/- .0005
ANGLULAR +/- 1/2-DEGREE

I have always been a proponent to adding an 'equal' sign so that such a block would read......

FRACTION = +/- 1/64
2 PLACE = +/- .015
3 PLACE = +/- .005
4 PLACE = +/- .0005
ANGLULAR = +/- 1/2-DEGREE

And, given that the decimal equivelant of 1/64th is .0156, I would recommend altogether that you remove the fractional requirement as you basically have it covered with the two place decimal tolerance of +/-.015. (You will also be doing your design crew a HUGE favor in that they will not have to constantly be resetting their CAD system back and forth between decimal and fractional systems between dimensions)
A huge timesaver!

My guess is that this also represents a migration of sorts for your company from fractional to decimal dimensions. I've been there, done that. Have some decimal equivelant charts handy for those that are less apt to figure this out on their own.

1. Drop fractional dimensions and tolerances altogether
2. Use the '=' sign in the tolerance as noted above.

and finally from the Department of Redundancy Department
3. Change 'Unless Otherwise Specified' to 'Unless Specified'

Couple of other title block suggestions....
A. Add 'Dimensions are in inches' (assuming you use inches)
B. Reference in the title block ANSI Y14.5 (if that is the standard you are using)
C. Add a small title block note stating that the drawing is in third angle projection along with a little truncated cone graphic.

Good Luck - Mousetrap

 

[imagitec]

I work for the American subsidiary of a German company in the semiconductor equipment industry, so we use metric, which I love from a computation point of view. Unlike Alexit, however, I do not love the default ISO tolerancing scheme. For those unfamiliar, the default tolerance depends on the magnitude of the dimension. As he indicates, there are actually three sets of possible defaults, fine (f), middle (m), or course (k). A note in the border specifies which one applies to the current drawing.

I find that even the fine defaults are inadequate, especially hole-to-hole dimensions over even relatively small distances (400 mm using fine tolerances and 120 mm using coarse). Perhaps they were developed for an industry with a different concept of "fine", like the automotive industry. Conversely, the default tolerances for small dimensions can be too tight. If the nominal thickness of a part is 6 mm, the fine tolerance is +/-.05mm (2 mils) and the coarse is +/-0.1mm (4 mils).

I would have to override virtually every dimension to produce an adequate drawing using this standard. I've worked with drawings from several European companies, and none of them do so. This fails to communicate design intent to the machinist and leaves you on shaky ground if the parts don't go together. This is an abdication of the engineer's responsibility (this happens in the US, too, with every dimension a baseline with the same precision).

Rob Campbell

 

[imagitec]

I agree that default tolerances should be different for different manufacturing processes, e.g. sheet metal versus machined parts, but I don't think the place to specify the difference is in the title block. There should be one default set of tolerances, with the caveat "unless otherwise specified". If the default tolerances are appropriate for a machined part but the current part is sheet metal, a set of defaults appropriate for a sheet metal part should be specified in the notes, with the same caveat. Tolerances applied directly to a dimension override everything else.

In the title block, and usually in tiny type, is too inconspicuous of a place to make this distinction. There are two chances for error: the engineer/designer/drafter forgets to make the change; or the machinist doesn't notice. If the machinist misses it and the parts don't go together, technically it isn't your fault, but that doesn't make the parts fit. The same thing can happen if the changed tolerances are specified in a note, but it's less likely.

Rob Campbell

 

[mkenwort]

.XXX = +/- .010
.XX = +/- .03
.X = .1
Angles = +/- 2 deg.

take it for what it's worth

other standards per mil-dtl-31000

 

[mkenwort]

forgot to mention, that's for aircraft engine externals industry, generally a great deal of cast parts that are machined to finish

good luck

 

[diamondjim]

Your mode and method of manufacture
should determine the general title
block tolerances like others have
mentioned. Your shop should be able
to tell you what they are capable of
manufacturing by the different processes
of manufacturing. Some tolerances are
very well defined by industry as to hole
sizes by standard drills etc. Turning,
grinding, milling, etc. all have their
own limitations. Weld dimension might
be quite gross unless you are fixturing
parts. If you are forming parts such
as forgings, ie. not machined, you would
also expect vary large variation in surface
dimensions again dependant on sizes.
You as the designer must work out with your
customer and your cost department the cost
of holding the closer tolerances if needed.
I like Mousetrap's comments the best if you
are speaking of machined tolerances on small
parts ie under 6 inches. Some european
companies show graduated tolerances based
on distances and also whether rough or finish
maching. Machineries Handbook does show
expected finishes by the different processes
of manufacture and this also determines the
extent of tolerance variation as well as distance
or length.

 

[chicopee]

fractional +or-1/64
two place decimal +or-.01
three place decimal +or-.005
four place decimal +or-.0005

 

[grogan5]

Unless otherwise noted:
- FRACTIONAL +/-1/64
- 2 PLACE DECEIMAL X.XX +/-.010
- 3 PLACE DECEIMAL X.XXX +/-.005
- 4 PLACE DECEIMAL X.XXXX +/-.0005
- ANGLES +/- 1/2 Degree

Been the standard I have used in Mechanical design since college, 25 years.

 

[toolmantwo]

OK people, I use the same as Grogan5 except for angles we use +/- 1 Degree. Our one place decimal is also +/- .015. Our internal shop people do not like us to use fractions, because they do not show up on the Calipers, and they will need to look up the conversion. We try to appease them some, but speed of reading is better in fractions I think.

What do you use for Metric systems in the Title block tolerances?

If you have metric dimensions and imperial system (inch) screw threads will you express the pitch diameter in metric or inch? Likewise for hole depths expressed in metric or inch?

Thanks, John

 

[yates]

Sorry to be picky folks, but what's all this about 'decimal places' I can understand the boilerplate tolerances varying with the number of 'significant figures' in the dimension, but not with 'decimal places'. How would you feel if a 0.002 dimension was given a 0.005 tolerance, as most of you are suggesting ?