Tolerance, Bilateral vs Limit
Close
Login to Your Account
Page 1 of 7 123 ... LastLast
Results 1 to 20 of 131
  1. #1
    Join Date
    Dec 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default Tolerance, Bilateral vs Limit

    Hey all! I was impressed with the answers to my last question, so I am back.

    Another topic discussed is how to dimension a feature on a part, for example a shaft of nominal diameter 5.000". I am using RC4, so the shaft is to be made with -.0016 to -.0032 as a tolerance. I have up to this point used bilateral dimensioning. I realize the machinist has to do the math on the 5.000" number to get the numbers to manufacture too. If I were to use limit, the numbers on the print would read 4.9984"-4.9680". Again, the machinist would have to do math if wants to hit mean. What do you guys prefer?

    Now, to throw in an additional argument. When I model this part in solidworks, I dimension the part to the nominal 5.000". I have read some places will actually put the mean dimension in the model, so in this case 4.9976". The print will then either read a symmetric +/-.0008 or do the limit again. The reason they do this is because we now have the CAM software that will import the model. If the model is made to that mean dimension, the programmer will not have to make any changes.

    I do not know any CAM software, how it works or how much work these different cases put on the machinist/programmer. So that is essentially my question, what makes it easier on others? I know if someone is measuring it is easier to see limit dimensions as that is the output on the caliper without any math.

  2. #2
    Join Date
    Mar 2014
    Location
    Nebraska
    Posts
    370
    Post Thanks / Like
    Likes (Given)
    42
    Likes (Received)
    232

    Default

    If you expect them to machine it drom the solid model, draw it the size you want it (the mean). If you expect them to make it from a print you can do it any way you like.

    You will run into problems (especially on turned parts) if the same tool is machining a feature that has an equally tight tolerance, only in the other direction.

  3. Likes toolsteel liked this post
  4. #3
    Join Date
    Feb 2016
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    189
    Post Thanks / Like
    Likes (Given)
    436
    Likes (Received)
    101

    Default

    The response is usually pretty good when you ask well written and thought out questions.

    Most of the folks I've talked to prefer limit dimensions for ease of use, so I try to give them that when I can. If you know it's going to be programmed and run through a CAM system, you can model it as nominal in Solidworks and then adjust the dimensions to read as limits. Best of both worlds, but takes a few more clicks.

  5. Likes toolsteel liked this post
  6. #4
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    535
    Post Thanks / Like
    Likes (Given)
    257
    Likes (Received)
    421

    Default

    Always always always always create the model to perfect form. You can call out the tolerances in the drawing however you want (we prefer symmetric bilateral). The point is some CAM guy is going to, at some point, pull the model in and never look at the drawing. Don't laugh, I've seen it happen.

    Drawings and models are a form of communication, your goal is to communicate as clearly as humanly possible. Having someone do extra math is just not good practice.

    Seeing 5.000 -0.016/-0.032 drives me up a wall. Yes the dim is 5 nominal. Is the part going to be used nominally? No. Then write the damn thing 4.976 +/-0.008 and be done with it.

  7. Likes Chris59, RJT, kenton, mountie, millNchill and 8 others liked this post
  8. #5
    Join Date
    Feb 2013
    Location
    Madison, WI
    Posts
    1,029
    Post Thanks / Like
    Likes (Given)
    1137
    Likes (Received)
    673

    Default

    Quote Originally Posted by Rewt View Post
    Always always always always create the model to perfect form. You can call out the tolerances in the drawing however you want (we prefer symmetric bilateral). The point is some CAM guy is going to, at some point, pull the model in and never look at the drawing. Don't laugh, I've seen it happen.

    Drawings and models are a form of communication, your goal is to communicate as clearly as humanly possible. Having someone do extra math is just not good practice.

    Seeing 5.000 -0.016/-0.032 drives me up a wall. Yes the dim is 5 nominal. Is the part going to be used nominally? No. Then write the damn thing 4.976 +/-0.008 and be done with it.
    This. It pisses me off when a model isn't to "perfect" form. It makes extra work for the programmer and/or machinist.

    Is there a reason not to do it this way?

  9. Likes mhajicek, npolanosky, toolsteel liked this post
  10. #6
    Join Date
    May 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    2,296
    Post Thanks / Like
    Likes (Given)
    204
    Likes (Received)
    1257

    Default

    Why wouldn't it be made to true size? That's just asking for a fuck up...

    I
    realize the machinist has to do the math on the 5.000" number to get the numbers to manufacture too. If I were to use limit, the numbers on the print would read 4.9984"-4.9680"
    That's a hell of a tolerance.

  11. #7
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,220
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2654

    Default

    i would never ever trust solid model. i always go off of drawing dimensions and tolerances. parts have to fit together. that is if shaft goes in hole it needs to happen. assembly guy not going to care about theoretical discussions.
    .
    things out of round (warpage), bores that have taper from tool wear, alot of things can cause problems.
    .
    worse thing in my experience is solid model with small corner radius or chamfers. if not selected correctly often program is .010" off if hard to see corner radius was .010", i would never trust solid model. i have seen too many small CAD problems become big problems making the part and assembling the part.

  12. Likes millNchill liked this post
  13. #8
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    535
    Post Thanks / Like
    Likes (Given)
    257
    Likes (Received)
    421

    Default

    Quote Originally Posted by AARONT View Post
    This. It pisses me off when a model isn't to "perfect" form. It makes extra work for the programmer and/or machinist.

    Is there a reason not to do it this way?
    We have some tooling made in Italy that completely ignores things like dowel fit. They draw it straight up line to line. Both the dowel and the hole to nominal. Clearance for cutting steels the same way.

    I have no idea how they finished the dies.

  14. #9
    Join Date
    Jan 2009
    Location
    Maine, USA
    Posts
    202
    Post Thanks / Like
    Likes (Given)
    97
    Likes (Received)
    90

    Default

    I agree with three posts above me. 5.000 (-x, -y) is not a proper tolerance. -0, +x or -x, +0 are appropriate for showing either side of nominal on a drawing. Also, ignoring the incorrect math in your first post, you wouldn't write (upper limit-lower limit), it'd be the opposite.

    A fit is a fit and a tolerance is a tolerance. In this case you can't combine them in my opinion.

    As far as modelling, I do not know, but it would never seem to be a good idea to model the part as something outside the tolerance of the actual part. Again, fit is fit and tolerance is tolerance.

  15. #10
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,220
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2654

    Default

    some will dimension a bore as 3.0000 +.0020/-.0000
    .
    cause bore needs to be big enough to get the mating part to fit into the bore. so everything dimensioned from that point of view or way of thinking
    .
    same with setting a indicating bore gage. do you set in middle of tolerance (looking for +/-.0010" or do you set 0.0000 at minimum size so bore gage reads +.0001 to +.0020"

  16. #11
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,640
    Post Thanks / Like
    Likes (Given)
    1222
    Likes (Received)
    2603

    Default

    I don't care really. But it has to be right.

  17. #12
    Join Date
    Dec 2016
    Country
    UNITED STATES
    State/Province
    California
    Posts
    152
    Post Thanks / Like
    Likes (Given)
    24
    Likes (Received)
    44

    Default

    Always model at nominal! I've seen minus/minus tolerances screwed up more times than limit dimensions.

  18. Likes mhajicek, Chris59 liked this post
  19. #13
    Join Date
    Dec 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Thanks for the replies everyone, and I apologize for typing the incorrect number in there.

    JCByrd I thought it was always upper limit, -.0016, and then lower limit, -.0032. That was my interpretation.... and never mind, as I type this I am reading ASME Y14 2.2 direct tolerancing and in that form that I have it typed out in, single line, it should be lower limit than high limit. This is what I really meant to have that look like (as looks in drawing with bilateral):
    (blank space)-.0016
    5.000
    (blank space)-.0032

    wasn't letting me use spaces!

    Thanks again everyone!

  20. #14
    Join Date
    Dec 2015
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    437
    Post Thanks / Like
    Likes (Given)
    144
    Likes (Received)
    251

    Default

    that looks like a very dangerous way to show the tolerance. Of course there are minuses in front of both tolerance limits but I could see very easily miss reading that as 5.000 +.0016/-.0032.

    I am defiantly in the model to nominal camp. I have a group that routinely brings turning me models with with a -.002/-.004 tolerance that is next to a chamfer with a angle call out up to a defined dia. Then the next dimension starts at the top of the chamfer meaning that the solid model is nothing like what they will get will get if I follow the dimensions. So every time I call them down to have them explain what dimensions are actually important and I usually end up not being able to use the solid model for anything.

    TLDR: Model doesn't match the dimension which makes me angry and wastes time.

  21. Likes millNchill, Chris59, mountie liked this post
  22. #15
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,640
    Post Thanks / Like
    Likes (Given)
    1222
    Likes (Received)
    2603

    Default

    Nominal isn't a word we should be using really.

    Nominal- adjective- .
    (of a role or status) existing in name only.

    I understand what it implies in Manufacturing. But if we're going to have a conversation about how to tolerance a part Nominal makes it even more confusing. Example; one person means Nominal as the exact dimension desired, another person means the whole rounded value. (5, in this case).

    IMO, none of it matters. The person looking at the Print needs to read it and understand it. If they fuck up, okay. If the Spendgineer fucks up, that's on them.

    R

  23. #16
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    1,087
    Post Thanks / Like
    Likes (Given)
    1346
    Likes (Received)
    735

    Default

    I've seen far too many cases where single sided tolerances end up defining impossible geometry, especially when the "nominal" size is outside the tolerance range. Model it at the median and call it 4.9976" +/- .0008", since that's what you really want. The programmer will program to the median, the operator will adjust to the median, the inspector will inspect to the median. Calling it anything else just adds more work for everyone (including redrawing geometry for the programmer) and adds risk of math errors and reading errors, such as the one you made in your original post (5.000" -.0016 to -.0032 is not 4.9984"-4.9680".)

    This may not be a big deal if you're just turning and/or grinding a plain shaft, but when it comes to shafts machined as bosses on milled parts and controlled radii and blends between the shaft surface and other features it can be a big deal.

    Calling it 15.0000" -10.0016 to -10.0032 is as meaningful to me as 5.0000" -.0016 to -.0032.

  24. Likes Rstewart, precisionmetal, Lewie, mountie liked this post
  25. #17
    Join Date
    May 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    2,296
    Post Thanks / Like
    Likes (Given)
    204
    Likes (Received)
    1257

    Default

    If I got a drawing that had a double minus or plus dimension I'm going to assume it's a mistake and have the engineer verify it. Then I'd probably have choice words for him/her.

    At work we work to models, very few drawings exist.

  26. #18
    Join Date
    Feb 2013
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    692
    Post Thanks / Like
    Likes (Given)
    145
    Likes (Received)
    740

    Default

    When I was an engineering manager, I passed a rule that everything was modeled at "nominal" dimension and all tolerances were bilateral/ symmetric. As far as I recall, this never caused any issues in the supply chain. I still model everything like that, and I look down upon any print that is toleranced any other way. I think it just shows laziness on the part of the designer/ drafter.

    And yes, I am one of those lazy/ ignorant people that rarely look at the print and run everything through a CAM system. Sure, I'll glance at the print and check for weird or extremely tight tolerances. Then I program everything off the model, check key dimensions and ship the part. My customers use me because I build difficult parts extremely quickly, often times overnight. I tell them that the model is the gospel with the print only being used for the tolerances that aren't easily elucidated by the model.

    I have a pretty refined system of programming and most errors can be prevented using verify on the CAM system. Programmed correctly, deviations only occur due to loading an incorrect tool or offset, excessive deflection in the part or the tool, parts being loaded incorrectly... I'm over simplifying of course, but I am just pointing out that parts that are correctly modeled to a nominal dimension are much easier to manufacture using today's technology.

  27. Likes Job Shopper TN, Rewt liked this post
  28. #19
    Join Date
    Jun 2006
    Country
    UNITED STATES
    State/Province
    Alabama
    Posts
    1,883
    Post Thanks / Like
    Likes (Given)
    1089
    Likes (Received)
    738

    Default

    Quote Originally Posted by G00 Proto View Post
    When I was an engineering manager, I passed a rule that everything was modeled at "nominal" dimension and all tolerances were bilateral/ symmetric. As far as I recall, this never caused any issues in the supply chain. I still model everything like that, and I look down upon any print that is toleranced any other way. I think it just shows laziness on the part of the designer/ drafter.

    And yes, I am one of those lazy/ ignorant people that rarely look at the print and run everything through a CAM system. Sure, I'll glance at the print and check for weird or extremely tight tolerances. Then I program everything off the model, check key dimensions and ship the part. My customers use me because I build difficult parts extremely quickly, often times overnight. I tell them that the model is the gospel with the print only being used for the tolerances that aren't easily elucidated by the model.

    I have a pretty refined system of programming and most errors can be prevented using verify on the CAM system. Programmed correctly, deviations only occur due to loading an incorrect tool or offset, excessive deflection in the part or the tool, parts being loaded incorrectly... I'm over simplifying of course, but I am just pointing out that parts that are correctly modeled to a nominal dimension are much easier to manufacture using today's technology.
    That's pretty much how I go about most things that come across my desk

  29. #20
    Join Date
    Sep 2010
    Location
    india
    Posts
    1,260
    Post Thanks / Like
    Likes (Given)
    73
    Likes (Received)
    229

    Default

    Targeting the mid dimension seems to be the most logical, as it will take care of variations due to random reasons. However, there was an argument some time back that since the tool wears out with time, resulting in increased size, the same tool can be used more often if we target a dimension lying towards the lower size.

  30. Likes 75sv1 liked this post

Tags for this Thread

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •