×
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

Anyone ever see a double positive tolerance?
6

Anyone ever see a double positive tolerance?

Anyone ever see a double positive tolerance?

(OP)
Anyone ever see a double positive tolerance?  (e.g 1.000 +0.005 +0.008)

I've always thought the target value must be between the maximum and minumum value; and was selected by the engineer based on maximizing yield depending on how the part would be made, and on maximizing performance of the final assembly.   The tolerances could be symmetric +/- 0.003, or they could be asymmetric +0.003 - 0.000, but I've never seen double positive tolerance, or double negative before.

Did I miss something in GD&T class?

RE: Anyone ever see a double positive tolerance?

Usually double positives and double negatives are used for fits (i.e. slip, locational, press, etc.)

I use them all the time.

Try to search before posting. This has been discussed before.

Here's on example.

http://www.eng-tips.com/viewthread.cfm?qid=212575&page=8

V

RE: Anyone ever see a double positive tolerance?

I've seen them.  I don't like them.

RE: Anyone ever see a double positive tolerance?

I start seeing them towards the end of the day.

I agree with the others.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 08
ctopher's home (updated Aug 5, 2008)
ctopher's blog
SolidWorks Legion

RE: Anyone ever see a double positive tolerance?

It never isn't done like that here... but if a double negative is actually a positive... then isn't a double positive actually a negative???
   

RE: Anyone ever see a double positive tolerance?

I've used them when I want to convey different information to different groups of readers, e.g. that the shaft takes a 120mm bearing, but it's pressed on.

It usually results in a call from the shop ("Am I understanding this correctly?" ... or some rude equivalent).  

It's not a bad way to:
- get acquainted with the guys in the shop.
- find out they are really working on your project.

 

Mike Halloran
Pembroke Pines, FL, USA

RE: Anyone ever see a double positive tolerance?

I'm not that crazy about them, but they do show design intent.

Joe
SW Office 2008 SP4.0
P4 3.0Ghz 3GB
ATI FireGL X1

RE: Anyone ever see a double positive tolerance?

Double positive (or negative) are part of comprehensive systems for limits and fits.  For example, the ISO 286 ISO system of limits and fits series provides for parts that can be designed with any combination (double positive, double negative, symmetric +/-, etc.).

You can review information on this subject here:

http://www.roymech.co.uk/Useful_Tables/ISO_Tolerances/ISO_LIMITS.htm

Regards,

Cory

Please see FAQ731-376: Eng-Tips.com Forum Policies for tips on how to make the best use of Eng-Tips Fora.

RE: Anyone ever see a double positive tolerance?

I've used double positive and double negative.  sometimes for fits, sometimes because a solid model hasn't been updated to have a nominal within the desired tolerance range on the drawing (yes, there are reasons to do this).

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

RE: Anyone ever see a double positive tolerance?

I agree with above that you see them a lot with shaft fits, especially ISO ones.

By extension some German drawings seem to use them even on items that aren't a classic 'fit' situation.

They can cause confusion so I avoid them.  Also with some CAD systems it can be awkward to achieve.

KENAT,

Have you reminded yourself of FAQ731-376: Eng-Tips.com Forum Policies recently, or taken a look at posting policies: http://eng-tips.com/market.cfm?

RE: Anyone ever see a double positive tolerance?

2
A lot of this stuff is very industry-specific.  I design custom assembly equipment for factory automation.  Unilateral tolerancing is really the only thing that makes sense in that context.  Check a catalog for dimensional drawings of anything - linear shafting, bushings, servo flanges, spacer blocks, dowel pins, raw steel dimensions... the list could go on and on.  If there's any sort of fit involved, you will see unilateral tolerances.  I'm constantly amazed at people's ignorance of this common practice.   

-handleman, CSWP (The new, easy test)

RE: Anyone ever see a double positive tolerance?

Mike's quote:

"It's not a bad way to:
- get acquainted with the guys in the shop.
- find out they are really working on your project."

I would add
 
- find out if they really read your drawings

RE: Anyone ever see a double positive tolerance?

Double positives or double negatives blow me away. One would still have to figure out the calculated nominal with both the USL and LSL. Why not just relay the true nominal with tolerances rather than making shop floor personnel use their calculators? It really seems like exercise in math but I am coming from a shop floor perspective.  

Dave D.
www.qmsi.ca

RE: Anyone ever see a double positive tolerance?

Most machinists are really good at giving what was asked for.  Even better if one asks nicely.  Double positive/double negative is not asking nicely.

I create part drawings that reflect the desired geometry of the part.  Things like sliding fit or other design intent information belong in the project design file, not on the drawing.

RE: Anyone ever see a double positive tolerance?

In places that are used to them I'm sure they're fine but places that aren't used to them they cause confusion.

On the other hand, places that are used to them can most likely handle nominals with +-, or max min, just fine.

So, unless I'm sure all potential users of the drawing are fine with them (not just now but in forseeable future) I'll convert to either limits or nominal with +-.

KENAT,

Have you reminded yourself of FAQ731-376: Eng-Tips.com Forum Policies recently, or taken a look at posting policies: http://eng-tips.com/market.cfm?

RE: Anyone ever see a double positive tolerance?

As I said, much of this stuff is pretty industry-specific.  I've never had a machinist from any shop we use complain about a double positive or double negative tolerance.  If I modeled everything at the middle of the tolerance range, my assembly drawings would look messy - two lines so close that they look like one thick line, ugly dimensions like 29.95, etc.   

-handleman, CSWP (The new, easy test)

RE: Anyone ever see a double positive tolerance?

(OP)
Thankyou,  And thank you for the link to the previous discussion.  

I hadn't seen the practice before and I didn't remember the practice being part of Y14.5.  I thought that the target value was an important piece of information for the machinist; tolerances could be, and in some situations should be, asymmetric, but the target dimension was an important piece of the design.  

OTOH I could see that if you just roughed all the dimensions in at 'nominal' and then just loaded the values from the ANSI B3.17 (Shaft Dia and Housing Bore) tables at the time you create the dwg, it could save engr time.  It is the equivalent of using MAX/MIN dimensioning. The machinist then choses the target value based on the processes being used.   
 

 

RE: Anyone ever see a double positive tolerance?

Jaimes, like folks above have mentioned it's more of an ISO/European thing.  If you use 'common' basic sizes of shafts/holes then these correspond in many cases to commonly available tools.  At least that's the theory I was told.

I don't believe it's in ASME Y14.5M-1994, though I dont' think 14.5 forbids it either.

KENAT,

Have you reminded yourself of FAQ731-376: Eng-Tips.com Forum Policies recently, or taken a look at posting policies: http://eng-tips.com/market.cfm?

RE: Anyone ever see a double positive tolerance?

dingy2,

   If the guy on the shop floor has a DXF file and is programming a CNC machine, it might help to see what the actual as-drawn feature size is.  

   I try to remember to convert my +/+ dimensions in SolidWorks to limit dimensions.  Either way, the CNC programmer has to pay attention.

                         JHG

RE: Anyone ever see a double positive tolerance?

29.95 is not nearly as nice as 30.  29.9865±0.0135 is downright hideous compared with 30g6.

-handleman, CSWP (The new, easy test)

RE: Anyone ever see a double positive tolerance?

Oops, should have been 29.9865±0.0065

-handleman, CSWP (The new, easy test)

RE: Anyone ever see a double positive tolerance?

Depends who's using it.

I know plenty that 30g6 would be meaningless to, especially without the relevant ISO referenced on the drawing.

KENAT,

Have you reminded yourself of FAQ731-376: Eng-Tips.com Forum Policies recently, or taken a look at posting policies: http://eng-tips.com/market.cfm?

RE: Anyone ever see a double positive tolerance?

Exactly my point (well one of my points anyway smile Dang shotgun brain), KENAT - depends on who's using it.

I do usually include the -0.007/-0.020 values along with the tolerance class.  

Also, from what I understand, the machinist will not be aiming at 29.9865 anyway.  If it's a shaft, he'll shoot for just under MMC.  Lots easier to fix if he misses.  It's easier to get to 29.993 by subtracting 0.007 from 30 than by adding 0.0065 to 29.9865.

-handleman, CSWP (The new, easy test)

RE: Anyone ever see a double positive tolerance?

I also don't like the idea of creating a feature in CAD with a size that is outside of its tolerance band.  As was discussed above, it can cause problems when cutting parts directly from CAD data.  Sure, the programmer should always double check, but "should" is a word that can waste a lot of time and money if used too liberally.

RE: Anyone ever see a double positive tolerance?

Quote: 29.95 is not nearly as nice as 30.  29.9865±0.0135 is downright hideous compared with 30g6.

If you put 29.9865±0.0135 on the drawing you have to have a gage that is accurate to .00005 which is pretty near impossible.  Any machinist that is not familiar with the ISO system of fits should not be making your parts.  Normally parts requiring these levels of precision are not going to be made by the illiterate.  If they are being made in volume there are probably automatic gaging systems in place with nice green & red lights that anyone can understand.

However, if you don't need asymmetric tolerances, definitely don't use them.

RE: Anyone ever see a double positive tolerance?

"Any machinist that is not familiar with the ISO system of fits should not be making your parts. "

Having picked my self up from the floor where I'd fallen laughing.  For those of us not caught up in the big defense & automotive supply chains, but too big to have much say in who the parts get sent to, I'd be amazed if Purchasing/QA even considered that issue.

Even in the UK we rarely used the "30g6" form, we'd put down the equivalent dimensions.  Only exception I can think of is for threads.

KENAT,

Have you reminded yourself of FAQ731-376: Eng-Tips.com Forum Policies recently, or taken a look at posting policies: http://eng-tips.com/market.cfm?

RE: Anyone ever see a double positive tolerance?

I've used them quite a bit but I've since replaced them with limits. Mainly because I got tired of machinists either calling asking if this is a typo and do I really mean +xx/-xx or, even worse, assuming that it is a typo and I get bad parts. It just wasn't worth the hassle.  

RE: Anyone ever see a double positive tolerance?

ctopher:

I have a bit of a problem with the web site you suggested when positional tolerances are called "true position". ASME Y14.5M-94 states that per 1.3.36 on page 4 True Position means "The theoretically exact location of a feature established by basic dimensions." The term used should have been "positional".

I might be nit-picking but a suggested web page and training advertisement should use the correct terms to gain credibility.  

Dave D.
www.qmsi.ca

RE: Anyone ever see a double positive tolerance?

Dave,

I don't back any site personally or professionally, I just suggest some sites for reference occasionally. Engineers should 'always' refer to ASME Y14.5-94.

I don't always have the ASME spec in front of me because I'm either virtual or at another site. So, I usually just do a quick Google search and share some sites I think may help a little.

I agree with you they should use the correct terms. But unfortunately I sometimes don't have the time to peruse the sites first.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 08
ctopher's home (updated Aug 5, 2008)
ctopher's blog
SolidWorks Legion

RE: Anyone ever see a double positive tolerance?

Off topic for this post, but "True Position" suggests your dealing with an old guy. i.e. thinking pre 1974.

On topic: ++ or-- tolerances are fine for fit tables, but I would never use them on a drawing. I either convert to limit dimensions or mean value with ± tolerance.  

RE: Anyone ever see a double positive tolerance?

I totally agree with handleman here.

"Check a catalogue for dimensional drawings of anything - linear shafting, bushings, servo flanges, spacer blocks, dowel pins, raw steel dimensions... the list could go on and on.  If there's any sort of fit involved, you will see unilateral tolerances.  I'm constantly amazed at people's ignorance of this common practice."

The whole or should that be hole reason behind this is to standardise things so parts are readily available and interchangeable, if you accept that all these items and more have unilateral tolerances on them why should the parts that they fit not have as well? The other option is of course to make everything specials and increase your costs by about 400%.

If you work in a part of the world that does not understand what 30g6 means then by all means put 30 -0.007/ -0.020 but to put 29.9865 +/- 0.0135 is just plain madness as you are just increasing the cost for producing the part with no gain what so ever.

I to am constantly amazed at people's ignorance of this common practice, I am even more amazed that companies that are forced to increase their costs through not understanding them still remain in business, they wouldn't be here next month in automotive.
 

RE: Anyone ever see a double positive tolerance?

Hey, thanks for fixing my spelling of catalog(ue)...I fear I am a poor user of the Queen's English.  winky smile

-handleman, CSWP (The new, easy test)

RE: Anyone ever see a double positive tolerance?

Writing the peasants english, "catalog" is just fine.

I'm contracted to a company where the division DRM disallows unilateral dimensions on drawings.

We must use "target" (i.e. mean) dimensions with ± tolerances; equal, or unequal, but no + or - 0.
 It is a shop, inspection driven requirement, much to the dismay of engineering.

Zero position tolerance an exception, of course.

RE: Anyone ever see a double positive tolerance?

"If you work in a part of the world that does not understand what 30g6 means "

ajack, in the UK we had people that couldn't handle this so used to normally put limits.

KENAT,

Have you reminded yourself of FAQ731-376: Eng-Tips.com Forum Policies recently, or taken a look at posting policies: http://eng-tips.com/market.cfm?

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