×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Tolerances on Mech Drawings
9

Tolerances on Mech Drawings

Tolerances on Mech Drawings

(OP)
Many years ago when I took a HS course in mech. drawing, the correct way to show dimensional tolerances was to have the same number for the + and -  eg., if you want something between 7 and 9 in. long you used 8+/- 1 (I can't figure out how to get the + directly above the - here).

But the foreign co. (Italian) I'm working at has a weird (to me) way of showing them.  They'll use anything from 7 +2/-0  to 9 +0/-2.  They've even used (I am NOT making this up!) something like 6 +1/+3!!!  This is not a small company, but a fairly large but old manufacturer of BIG equipment.

Anyone seen anything like this before?

RE: Tolerances on Mech Drawings

yeah, I see it all the time.  check out ANSI standard limits and fits for examples (machinery's handbook).

There are plenty of reasons why you would want to use unilateral tolerances, but most of them come down to ease of reading or ease of checking.  If you have a hole that's specified as x -0/+tol, and a shaft that's specified as x -tol,+0, then you can easily see that they will have, at MMC, an exact match in size.  

RE: Tolerances on Mech Drawings

Warning! rant.mode = true

8 +1/-1 is not necessarily the same as 7 +2/-0, or 9 +0/-2.

The problem with tolerances is that nobody bothers to consider the root of the word.  Tolerance comes from tolerate.  The whole point is to define how much ERROR from the ideal case can be tolerated by the design.

I often hear "Well the parts don't go together right because there was an accumlation of manufacturing tolerances."  WRONG!  The purpose of actually thinking about, and correctly defining tolerances is to ensure that the inevitable manufacturing ERRORS will not result in parts that don't go together.

rant.mode = false

RE: Tolerances on Mech Drawings

Tpically the number listed is the target number.  The tolerance gives the acceptable range.

See ANSI 14.7 for correct notation.

RE: Tolerances on Mech Drawings

2
The way how your Italian company shows the tolerances is nothing unusual in "metric" countries.
This way of tolerancing makes it easier for the designer do define the min. clearance/interference.
Say we have a shaft 50mm dia and we want a bore locate on it with the min. clearance of 0.1mm and the machining total tolerance for both parts 0.05mm.
The "metric way" to dimension it would be:
Shaft dia 50 +0.0/-0.05
Bore dia 50 +0.15/+0.1
Locating smallest bore 50 +0.1) on largest shafts (50 +0) shows immediately the min. clearance.
The dia 50 in this example links the two parts together - it is usually called the "nominal" size for both of them.
This tolerancing style probably originated in the ISO system of fits( like 50H7/g6), what is used for decades and simplifies design, manufacturing and checking (if used properly).
Again - the main reason for doing it is to give to BOTH parts the same nominal size and using the tolerances define the fit. And for the ISO fits - there are standard tools, gages waiting for the smart user, it means less expensive tha the "special" gages/tools if no standard is used.

RE: Tolerances on Mech Drawings

ditto the previous posts, especially gearguru. I'm surprised Metalguy didn't mention tolerance designations like H7/g6.

One problem though is how do you represent the geometry with a tolerance (such as 50 +0.15/+0.1) with a CAD/CAM system?

Most CAD designers would model a shaft with the nominal diameter of 50. But this would be out of tolerance if the NC programmer only used the CAD geometry.

RE: Tolerances on Mech Drawings

The one thing they don't teach in mechanical drawing is, "What's a drawing FOR?".

A sketch can tell someone what you WANT.

A drawing tells someone what you WILL NOT ACCEPT.

;---

Asymmetrical tolerances are a shorthand way of saying that you'd prefer the feature be at the nominal location, but the design can tolerate (there's that word again) more varaition in one direction than another.

;---

Symbolic tolerance ranges are a shorthand way of dimensioning a joint for a particular fit, without going to the bother of calculating the numbers for every joint.  It makes a lot of sense, though I never got used to it.

;---

I've gone to the trouble of trying to include tolerances in CAD geometry.  It doesn't take a very complex part to drive you crazy, trying to figure out which line is the one you want to snap to, connect, etc.  The closest I've come in practice is to model tapped holes as a cylinder of the tap drill diameter, and clearance holes at their nominal drill size.

As for modeling a feature where the desired size is not on the nominal, i.e., the tolerance range does not include the nominal, I'm not sure what to do.  If you model the desired size, you have to override the dimension to show the nominal on a print, and if you model the nominal, the programmer has to work more carefully.  Either way is likely to cause an error sometime.  Modeling the nominal is slightly less likely to cause production of bad parts, but overriding dimensions carries risks of its own.

On the other hand, the number of times I've toleranced a part like that could be counted on the fingers of one hand, and it confused the hell out of everyone who saw the print.  If you want to know when your part actually hits the shop, that's one way to do it; the phone will ring for sure.



Mike Halloran
NOT speaking for
DeAngelo Marine Exhaust Inc.
Ft. Lauderdale, FL, USA

RE: Tolerances on Mech Drawings

(OP)
Thanks for all the good responses.  looks like the company is doing things correctly.

RE: Tolerances on Mech Drawings

Metalguy,

   My copy of Engineering Drawing by Thomas E. French, McGraw Hill, published 1941, shows +/+ tolerances.  They describe the practise as acceptable, but not as clear as limit tolerancing.  They discourage making the workman do arithmetic.  That makes the practise legal here in North America at least back to WWII.

   With CAD, there are several ways to model something to scale and apply dimensions and tolerances.  The nominal dimension, max and min allowance format makes clear what someone did.  If you are working on someone else's drawings, you could get a nasty surprise.

                                JHG

RE: Tolerances on Mech Drawings

Using the tolerances as metalguy asked about means, that the people using the drawings are properly trained. Unfortunately the US colleges do very little (if anything at all) to improve the situation.
For the CAD representation: in our company the models are always created using the mean dimensions (average between the upper and lower limits) even if they are dimensioned different way. This helps if the models are used for rapid prototyping or castings etc. Again - the drafter has to be trained how to calculate the mean dimension. In case of confusion - and ISO fits are confusing for most of them -they ask your truly...

RE: Tolerances on Mech Drawings

For those of you who need to "decode" some ISO metric fits withot looking in a book, here is the web address of the Fit Calculator. I mentioned it before, now I found the address.
Enjoy!

http://www.tecnologix.net/en/tools/passungsrechner...

RE: Tolerances on Mech Drawings

I do not know if you are talking
about acad or not, but for some
reason in order to get the plus
sign to appear, I would enter
1.00000001 for the plus tolerance
and 1 for the minus tolerance.
Then it would show the plus and
minus in the tolerance in the
dimension.

RE: Tolerances on Mech Drawings

tchettle,

   ISO fits are explained in the Machinery's Handbook.  The ANSI fits are based on ISO tolerance values, and are also based on the Machinery's Handbook.

   There ought to be a macro button on this site that automatically generates the reply "Refer to the Machinery's Handbook!".  

                       JHG

RE: Tolerances on Mech Drawings

I don't have Acad but in some cad programs you can enter Alt 241 and get the ±.

RE: Tolerances on Mech Drawings

UncleSyd, in AutoCad (any version) the command stroke on the keyboard is simply %%P.  Back in the day, AutoCad Version 8, keystroke entries where the norm.  I guess it just got built into the code somehow.

There are a ton of them, %%C for the diameter symbol, %%D for degrees, the list goes on.

I gotta admit, I never heard or seen +/+.

Kenneth J Hueston, PEng
Principal
Sturni-Hueston Engineering Inc
Edmonton, Alberta Canada

RE: Tolerances on Mech Drawings

I heard someone say that the drawing needs to minimize how much arithmetic the fabricator has to do.  NO!  That is part of the fabricator's job and it is expected that he will have to do it.

An engineering drawing exists for depicicting the end-item;  if a dimensioning and tolerancing style emphasizes the end-item's functional requirements while requiring the machinist to do some calculations then that's OK.

The drawing is an ENGINEERING tool that is used for inspection and for clearly protraying the end-item's functional requirements.

To be fair, though, the draftsman should never go out of his way to make a drawing that requires the machinist to figure things out!


Tunalover

RE: Tolerances on Mech Drawings

tunalover,

   I was quoting my 1941 drafting book.  I collect old books, especially engineering and history.

   The book actually is correct in the context of their discussion.  If I am working on a drafting board, the clearest way to express a tolerance is to show limits...

   1.253/1.251 DIA

   This is as clear an instruction as you can send to a fabricator, and it meets engineering requirements.

   In my next paragraph, I was somewhat vague, but the point is that with CAD, we use the scale drawing/model, and there are several ways of causing the display above.  This could be nasty if your job is to model and dimension the mating part.

   1.250 +.003/+.001 DIA shows the real diameter of the scale model.  It shows that I applied the ANSI fits and/or the ISO tolerances entirely with the dimensioning tool's tolerance feature.  At the preliminary phase of the design, I even use the ISO tolerance codes because they are independant of the dimension.  I have not the nerve to send these out to the fabricator.

   I tend to change diameters to limit dimensions when I finalize the drawings.  The toleranced dimensions are used mostly by the fabricators and inspectors.  Engineers can get at my CAD model.

                       JHG

RE: Tolerances on Mech Drawings

Typicall DrawOh, CAD models are drawing to maximum material.  In other words, given 1.253/1.251 as an outer diameter, I would draw a line at 1.253 diameter.  Conversely, given 1.251/1.253 as an inner diameter, the line would be drawn at 1.251 diameter.

There is nothing wrong with reporting 1.253/1.251, just as 1.252 dia +/-0.001, 1.251 dia +0.002/-0.000 or 1.253 dia +0.000/-0.002.  Depending on the circumstances of the design, the designer would make a consideration on what is theoretically needed to what is practically possible.  This in itself takes years of experience, although I have seen enough raw talent to have faith in the practice of engineering, as a skill and an art.

CAD drawings should show maximum material.  That way if buddy is having a bad day on the machine and overshoots the lower number, he has an upper target to meet knowing the piece is not dysfunctional.  Should he violate the limit, then I expect a visitor.

Kenneth J Hueston, PEng
Principal
Sturni-Hueston Engineering Inc
Edmonton, Alberta Canada

RE: Tolerances on Mech Drawings

We in design engineering preferred drawing to the
max material condition.  The shop insisted that we
draw to mean dimensions.  The shop won.  Both make
sense.    

RE: Tolerances on Mech Drawings

Quote:

...This way of tolerancing makes it easier for the designer do define the min. clearance/interference.
Say we have a shaft 50mm dia and we want a bore locate on it with the min. clearance of 0.1mm and the machining total tolerance for both parts 0.05mm.
The "metric way" to dimension it would be:
Shaft dia 50 +0.0/-0.05
Bore dia 50 +0.15/+0.1
Locating smallest bore 50 +0.1) on largest shafts (50 +0) shows immediately the min. clearance...

...the main reason for doing it is to give to BOTH parts the same nominal size and using the tolerances define the fit.

In this example the shaft is supposed to be 50mm diam.  So, I would just specify:

shaft: 50.0 +/- .025
bore: 50.15 +/- .025

This would also make sense, since the machining error is "random" and can be "+" or "-".  I assume this is why why fabricators would prefer mean tolerances.
Largest shaft (50.0+.025) in smallest bore (50.15-.025) shows min clearance of .1 as expected.

  

RE: Tolerances on Mech Drawings

   1.250 +.003/+.001 DIA shows the real diameter of _MY_ scale model.  I should have been clearer.  You guys are making my point.  There is more than one way to do this, including some dumb ways.  I have gone into AutoCAD drawings and found dimensions exploded and typed.  I guess the equivalent in SolidWorks would be to replace the <DIM> with text ("I'm in a hurry!").  I have not encountered this yet.

   I prefer to model at the exact nominal dimension.  The shaft and the hole are modeled at 1.250"DIA or 50mmDIA or whatever.  On my arrangements or assemblies, I make a note indicating an ANSI fit like RC4 or LC5, depending on my requirements.  Lately, I have been marking the ISO tolerance codes on my dimensions, making the tolerance independant of the current dimension.  Modeling MMC requires me to know what tolerance I am using, and I am not always sure of this until late in the design.  The ANSI and ISO tolerances vary with diameter.  At the end of the job, I fix everything to make it readable to the shop, since they are the primary users of the drawing.  I prefer to send drawings out to the fabricator, and I send DXFs if they ask me.  I have sent SolidWorks models to sheet metal shops.

   A corporate standard is desirable here.

                              JHG

RE: Tolerances on Mech Drawings

Quote:

In this example the shaft is supposed to be 50mm diam.  So, I would just specify:

shaft: 50.0 +/- .025
bore: 50.15 +/- .025

This would also make sense, since the machining error is "random" and can be "+" or "-".  I assume this is why why fabricators would prefer mean tolerances.
Largest shaft (50.0+.025) in smallest bore (50.15-.025) shows min clearance of .1 as expected.
-----------------------------------------------------------
I would agree with the above. I've been producing programs for milling and turning for over 10 years in the UK and we get drawing from all over the world.  

We always standise them to nominal with +/- tolernaces.

It is far easier to control in production for especially on milling out thin materials where we cut out circuits in one pass.

Regarding +/+ tolrances we see these a lot on features such as push fit holes for electronic components,  often drill diameters are specified 1.8mm Dia +0.02 / +0.5


RE: Tolerances on Mech Drawings

"tolerance designations like H7/g6."

"I heard someone say that the drawing needs to minimize how much arithmetic the fabricator has to do.  NO!  That is part of the fabricator's job and it is expected that he will have to do it."

"At the preliminary phase of the design, I even use the ISO tolerance codes because they are independant of the dimension.  I have not the nerve to send these out to the fabricator. "

"To be fair, though, the draftsman should never go out of his way to make a drawing that requires the machinist to figure things out!"
--------------------------------------

We used some moderately complicated power drawbars from a German company.  They called out their required fits as H7/g6, etc.  They also included a table translating those designators into real numbers.

I'll bet that saved a few re-works and non-value-added discussions about the difference between g6 and G6.
Well worth it.  





RE: Tolerances on Mech Drawings

We outsource fabrication to a rather long list of qualified vendors here in the USA.  Over time, the same part can be made by several different suppliers.  We provide SolidWorks models (or 3D translations; IGES, STEP, etc.) and minimally dimensioned drawings to them.  We receive better (more accurate) parts by modeling to the nominal/mean value and using symmetric tolerances as most of our suppliers CAM directly from our models.  Force fits (and a few other special cases) being exceptions to this general rule.  Fasteners and purchased hardware are always modeled at MMC.

For us, modeling/dimensioning a nominal value with either +/+ or -/- tolerances is the shortest path to rejects and scrap.  When the modeled geometry and/or dimensioned print show nominal values outside of the allowable tolerance range we often get what we modeled/drew instead of what we wanted.

RedPen





RE: Tolerances on Mech Drawings

I like to model at MMC nominal then use bilateral tolerance on the drawing to fit (i.e. shaft at 40 -.003/-.009 & hole at 40 +006/+012). This works with vendors that read the drawings and the guys using the model w/o checking the print still have enough stock to rework the parts when I send them back.

RE: Tolerances on Mech Drawings

I was trained to the ISO drawing standard, but through experience learnt that:
It is OK to specify H7/g6 - you only have to reject a part once and then everybody knows. Sounds harsh - but heck, my time costs more than the guy on the floor and hence I only need to communicate my design intention, in this case a close sliding fit.

Each workshop is different. You first have to understand how a part will be made, then dimension it. What works for one workshop costs time in another - they have different tools and techniques.

Drawing is the way we talk to the guys on the floor. While the correct way is to give only the minimum dimensions, the best way is give some reference dimensions and mark them as such - especially for fabrications.

If you get things done on contract you better tollerance properly or you will have no comeback. However, use realistic tollerances - or it can cost you heaps.
    

RE: Tolerances on Mech Drawings

As "BOO 1" correctly stated your dimension should be the target number. The tolerance is what size of deviation on both the plus side and the minus side creates an accptable part.

As far as how to show the tolerance formatted as you have asked depends on the cad system you use. I have SolidWorks. In the drawing mode it allows me to choose various methods of displaying the tolerance. You should choose according to your company standard if applicable, or whatever method most clearly shows your requirement for deviation.

RE: Tolerances on Mech Drawings

Dimensioning in this fashion is common to the company I work for when designing certain types of assemblies. We manufacture machine tools. Fits are very important and dimensioning in this way lets the machinist know what your intentions are.

For instance, lets say I wan't a cylinder assembly with a nominal bore of 10". I would dimension a class RC3 precision slip fit intended for a nominal diameter of 10 inches like this:

10.0 +.0020/-.0000" for the hole,
and 10.0 -.0025/-.0037" for the shaft.

This lets the machinist know immediately what the target assembly dimension is, in this case we are going for a nominal bore of 10.0".

The method that you are accustomed to would dimension these parts like this:

10.0010 +/-.0010" for the hole,
and 9.9969 +/-.0006" for the shaft

This would likely confuse our machinists as to what the intended result would be.

RE: Tolerances on Mech Drawings

I understand the usage of -/- tolerances, but feel that if the dwg and design are correct, the machinist doesn't need to know anything about the assembly.  I would use 10.0010 +/-.0010" for the hole and 9.9969 +/-.0006" for the shaft on the drawings.  If the part is machined to those dimensions, the assembly will work.

RE: Tolerances on Mech Drawings

Ehw I believe the +/+ and -/- dimensions came from the holes and shafts standards h7 and the like.

The reason for this is they are a standard so any shaft or bearing or anything from any manufacturer will give you a press fit, slide fit or whatever is required.

They are all based around a nominal size and the tolerances change as the nominal shaft or hole size changes. So to use your example it may do what you want but the hole would be in a different set of limits to the shaft, i.e. one is 10-15mm and one is 6-9 (the exact figures may not be correct) so your sizes would not fit say a h7 manufactured by another company.

Why change a standard that works perfectly well?

RE: Tolerances on Mech Drawings

ajack,
I guess I don't understand your point. As in the example above, I have a 10" nominal bore and need a class RC3 precision slip fit.  This calls for an H7 hole and an f6 shaft.
What is the difference if I dimension the hole 10.000 +.002/-.000" and the shaft 10.0000 -.0025/-.0037
vs
the hole 10.001 +/-.001" and the shaft 9.9969 +/-.0006"?The range of an acceptable part is the same, it is easier to accurately model, and those numbers mean the same thing anywhere in the world (as long as they understand inches;))
It shouldn't matter where I have it made, if it meets those tolerances, it will have a class RC3 slip fit and will work.

RE: Tolerances on Mech Drawings

The same for inspection. Won't inspectors measure the part the same in any case?
I am on ewh's side.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

RE: Tolerances on Mech Drawings

Having re-read what you said yes you are right it would be the same, however I still don’t see the point in going away from a standard that has been around for years and works fine, what is gained?

Maybe I am just being grumpy, I got home tonight to find my house had been broken into.

RE: Tolerances on Mech Drawings

That's too bad. I have an alarm, a dog and a gun. No break-ins yet. Hope all is well.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

RE: Tolerances on Mech Drawings

ajack,
I'm just going along with the times.  The classification system for fits is excellent for design.  However, in today's world, we have to document that design using solids on a computer.  It is much easier to see how a design works when you have the parts modeled at a size they will actually exist, and document it as such.  A +/+ or -/- tolerance adds confusion to this situation, i.e. a 10" nominal shaft should be modeled as it would be created, 9.9969 +/-.0006".
Sorry to hear about the break in.  That's enough to make anyone grumpy.

RE: Tolerances on Mech Drawings

Your points are all well taken. One point I should have mentioned really has to do with avoiding my own errors. My references on tolerances calls out nominal sizes with tolerances shown as I had posted, i.e. 10 -.0025/-.0037".

  If I was asked to dimension ouside of the standard it would require me to do a few calculations to convert the standard to a different system. This in itself could introduce error, especially towards the end of the day when I too am tired and grumpy . I appreciate that there are modelling systems that cannot handle this kind of tolerance, but I am a bit surprised that the newer software cannot.

RE: Tolerances on Mech Drawings

Maybe there are programs to handle it, but I am not familiar with them.  I do know that many do clearance analysis, but with a part modeled with a +/+ or -/- tolerance, the nominal size never exists.  Thus if modeled at nominal, a clearance analysis would not give you realistic results.  I guess you could edit the dimension on the drawing to reflect the nominal size, but this is usually not a good idea.  The dimension would lose it's associativity to the model, and would add another detail that anyone editing the model would have to be aware of.  I think that that would present more of a chance for error than converting the tolerance.

RE: Tolerances on Mech Drawings

I see your point ewh, the software we use does allow you to add hole/shaft sizes h7 etc, but only if you model to the nominal size, it would allow it for example on 10 but not 9.996. This obviously has plus and minus, no pun intended, as you can use the system that is standard and most (at least in automotive industries are used to) but does mean that everything is size for size, so as you rightly say does not show a clearance or drive between the two.

None of this really matters if everyone is on the same system, but becomes more of a problem when information goes through a translator, as text and annotation seem to be two of the things they (especially IGES) do not handle that well. As far as I am aware no system allows you to model intent, only text does this.

I wonder if we will have new standards in a couple of years as 3D becomes more and more the norm, probably driven by the largest supplier I guess Catia or Solid works or whether this will still be being debated in a couple of years time?

RE: Tolerances on Mech Drawings

ewh,
Curious on your opinion. For example, if a part is dim at 9.877 +000/-.002, would you model it at 9.877 or 9.876? I would use 9.876.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

RE: Tolerances on Mech Drawings

ajack,
I hope that softwares and translators will support ASME Y14.41-2003 DIGITAL PRODUCT DEFINITION DATA PRACTICES in the near future.  As it is, one of our customers (a major aeronautics company) has sent us files that approach ASME Y14.41, and almost all of the part info is in the 3D file.  What isn't in the part file is in text files.  All of the annotations and dimensions were converted to curves, and there are no drawings.  They look quite confusing (and intimidating) at first, until you understand how they are structured.
I don't see this standard getting a huge following for quite awhile, but it can streamline design and manufacture.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources