Page 3 of 7 FirstFirst 12345 ... LastLast
Results 41 to 60 of 121
Like Tree19Likes

Thread: Asymmetric tolerancing

  1. #41
    Join Date
    Nov 2005
    Location
    Maryland
    Posts
    7,072

    Default

    Quote Originally Posted by litlerob View Post
    ...we are going to try and make the part as easily and quickly as possible, so shooting for the middle of tolerance is what we as machinists are going to do.
    In the example shown, the nominal hole diameters are standard twist drills.

    If you shoot for the middle of the tolerance band, you would have to order custom-made drill bits in those adjusted sizes.

    Is that what you're proposing? It would significantly impact your cost of production.

    - Leigh

  2. #42
    Join Date
    Nov 2005
    Location
    Maryland
    Posts
    7,072

    Default

    Let me try to get this back on topic.

    If we were talking about a bored hole, I would agree that shooting for the mid or slightly smaller would be an appropriate programming approach.

    But this is not a bored hole, it's a drilled hole, designed to be done with standard twist drills, which seldom cut under-size.

    - Leigh

  3. #43
    SeymourDumore is online now Diamond
    Join Date
    Aug 2005
    Location
    CT
    Posts
    6,354

    Default

    Quote Originally Posted by The real Leigh View Post
    But this is not a bored hole, it's a drilled hole, designed to be done with standard twist drills, which seldom cut under-size.

    - Leigh

    Leigh

    I think we all understand what you're trying to say, but the designer is really not doing any favors for the machinist
    by specifying .250 +.01/-0 instead of .255 +/-.005 or .250-.260, or for that matter .250 with a UOS of .xxx - +/-.005.
    If you see any of the above, you will use a 1/4" drill to make the hole, and maybe use a reamer/endmill/special tool #5 to get it:
    a: within the tolerance band
    b: To a specific value within the tolerance band if needed for your subsequent operation


    The issue with the unilateral or assymetrical tolerances is that it in most cases someone will scribble the mean value on the print with a pencil, pen, magic marker or blood.
    No matter what, the end result will negate the original tolerance description.
    But for what it's worth, all of the above a peanuts and is easily resolved with a quick math either in your head or using a calculator. IOW it is a virtual non-issue.
    The real problem is when the drawings are received in a CAD format' let it be 2D or 3D solid, and the dimensions are drawn to nominal instead of mean.
    From my experience, no designer has a freaking first clue how much of a bitch that really is!!!
    They expect that quotes and prices to reflect the fact that they've helped you out by supplying electronic files by which your job is made easier.
    I do not care what CAM software you use, if all your models/geometry is drawn to nominal and some otherwise simlar features are +something/-nothing and +nothing/-something,
    there is no way to make your part properly without having to first scrutinize the CAD file and edit it if needed.
    It is very often the case that you have a .250 +.005/-0 and a .250 +0/-.005 feature on the same part, and both is drawn to .250.
    There is no possible way to make that part properly using CAM unless you edit the feature!!!

  4. #44
    Join Date
    Nov 2005
    Location
    Maryland
    Posts
    7,072

    Default

    Hi Seymour,

    This is one of the problems confronting modern manufacturing, and it's a difficult problem to solve.

    The parts in question have existed for well over 70 years, and have done quite credible service in literally millions of products.

    CAD and CAM present an interesting environment that can be entirely virtual, totally divorced from the real-world application.
    You can easily define a position, for example, relative to any other position in the model.
    The fact that the dimension cannot possibly be measured by any real tool to any significant degree of accuracy is totally lost on the mouse-pushers.

    - Leigh

  5. #45
    SeymourDumore is online now Diamond
    Join Date
    Aug 2005
    Location
    CT
    Posts
    6,354

    Default

    Quote Originally Posted by The real Leigh View Post


    The parts in question have existed for well over 70 years, and have done quite credible service in literally millions of products.

    While I can't speak for the other posters, I for one agree. The part has not only been designed long ago, but the process to make it is also
    defined in 10 ways to sunday.

    But as you say, it is the modern design practices that will need a serious look to to be defined to suit all, the design, manufacturability and implementation purposes.
    I could post a 3D solid in SW and the accompanying blueprint in a PDF form from a famous German maker.
    It has 178 measurement points, 37 of which is of the unilateral -/- and +/+ tolerances.
    Without actually supplying the files, please trust me, every one of those dimensions is drawn to the "nominal" values. Just by using the solid model, the part is/was
    not manufacturable without at least an hour of editing.
    I use Inventor, so had to go to a friend's place to edit it as I really wasn't up to recreating it natively nor use Fusion to dick with each and every one of the features.

  6. #46
    litlerob's Avatar
    litlerob is offline Hot Rolled
    Join Date
    Jun 2009
    Location
    PDX, OR
    Posts
    547

    Default

    Quote Originally Posted by The real Leigh View Post
    In the example shown, the nominal hole diameters are standard twist drills.

    If you shoot for the middle of the tolerance band, you would have to order custom-made drill bits in those adjusted sizes.

    Is that what you're proposing? It would significantly impact your cost of production.

    - Leigh
    Just re-checked the OP, personally I don't see any nominal drill sizes at all. That is not to say that I don't know which drills those are , but the way my mind works, I see the middle of tolerance +.0015/-.0. But maybe that's the subject of the thread huh?

    Robert

  7. #47
    jim rozen is offline Diamond
    Join Date
    Feb 2004
    Location
    peekskill, NY
    Posts
    21,601

    Default

    "explain to me,[...] how any conceivable unilateral tolerance could not be expressed in symmetrical terms."

    Obviously they *can*. Most machining operations produce a variation in part sizes that
    follow a gaussian distribution - the 'bell curve' that shows that most of the numbers
    will cluster around the center of the distribution. Hence the propensity for bilateral
    tolerancing in the industry.

    There may be a contingent here who believe in their heart of hearts, that by changing the
    way the tolerances are called out, will result in parts coming from manufacture with an
    altered distribution of sizes that no longer obey gaussian statstics. I assure you this
    is wrong.

    There is really only one way to produce a non-gaussian distribution of parts for the stak-on terminal.
    Put the nominal dimenesion exactly *at* the low limit for the hole size. Then discard any parts that
    size below the low limit - which will be about half of them, overall.

    This is actually how electronic resistors are graded. They're manufactured, then measured, and then
    the tolerance bands are painted on. This is why if you actually measure 20 percent, 10 percent, 5 percent,
    and two percent resistors, each set has a decidedly non-gaussian distribution! But if you put them all
    together in a bin, and measure *all* of them, they will have a gaussian distribution again!

  8. #48
    Join Date
    Nov 2005
    Location
    Maryland
    Posts
    7,072

    Default

    Quote Originally Posted by jim rozen View Post
    There is really only one way to produce a non-gaussian distribution of parts for the stak-on terminal.
    Put the nominal dimenesion exactly *at* the low limit for the hole size. Then discard any parts that
    size below the low limit - which will be about half of them, overall.
    Excellent example of how modern statistical methods and CNC mentality get in the way of good machine work.

    Twist drills do not cut undersize. If you use a drill of the proper size as stated, you get holes that will vary from that size to some amount larger.

    As a reference, AND10387 gives the tolerance for drilled holes in the range of 0.251"-0.500" as +.006"/-.001" (WOW, an asymmetric tolerance!).
    This is an Air Force-Navy Aeronautical Design Standard. But obviously they don't know what they're talking about.

    - Leigh

  9. #49
    barbter is offline Stainless
    Join Date
    Oct 2007
    Location
    UK
    Posts
    1,351

    Default

    Quote Originally Posted by The real Leigh View Post
    .......Twist drills do not cut undersize. If you use a drill of the proper size as stated, you get holes that will vary from that size to some amount larger.

    As a reference, AND10387 gives the tolerance for drilled holes in the range of 0.251"-0.500" as +.006"/-.001" (WOW, an asymmetric tolerance!).
    This is an Air Force-Navy Aeronautical Design Standard. But obviously they don't know what they're talking about.

    - Leigh
    Good call to use this tolerance for drills because TWIST DRILLS CAN CUT UNDERSIZE......(depending upon the mtl).

    I hate the + something - nothing tolerances, and everyone I know will always aim/make mid tolerance.
    If you have a shaft that is called 0.5 +.005/-0. , why would you try to make it 0.5? You're potentially putting it in the bucket, and even if you make it as close to 0.5000 as you can, they'll be a bloody inspector checking it scrapping it saying you're half a tenth undersize. Why risk it, unless you're mad.

  10. #50
    Join Date
    May 2007
    Location
    Munich, Germany
    Posts
    40

    Default

    Well maybe you could step a little back from your point of view one (!) drawing and try to understand the person who designed the whole assembly? Most nominal diameters are of round numbers or taken from standardised rows. This was chosen to make designing the machines that you work on, as well as the cars you drive more easy!

    "we'll take this 0,5 inch shaft, fit it in here and then..."

    the shaft will get a -/- or maybe -/0 tolerance because the bushings or the roller bearings are sold as + nothing/ +something. Could you immagine how much work it will take for an engineer to recalculate all the round nominals to mean nominals in one complete gear?

    Now could you brave machinists tell me in a sentence or maybe two what this whole 3 page thread is all about?

    I do know that an assembly/gear/machine I design will hardly have a dimension that will measure the way I have drawn it! But I surely have a reason for the min. and max. I have chosen by tolerance!

  11. #51
    SeymourDumore is online now Diamond
    Join Date
    Aug 2005
    Location
    CT
    Posts
    6,354

    Default

    Quote Originally Posted by benedict leighton View Post

    the shaft will get a -/- or maybe -/0 tolerance because the bushings or the roller bearings are sold as + nothing/ +something. Could you immagine how much work it will take for an engineer to recalculate all the round nominals to mean nominals in one complete gear?

    Now could you brave machinists tell me in a sentence or maybe two what this whole 3 page thread is all about?

    Sentence or two..... My own perspective:

    #1: """Could you immagine how much work it will take for an engineer to recalculate all the round nominals to mean nominals in one complete gear?"""
    Answ: So instead, the engineer delegates that work for the machinist.

    #2: """the shaft will get a -/- or maybe -/0 tolerance because the bushings or the roller bearings are sold as + nothing/ +something."""
    Answ: If you know that up front, then don't draw it to a + size when it will only fit on the - size. ( or the same for the opposite )

    #3:"""Most nominal diameters are of round numbers or taken from standardised rows. This was chosen to make designing the machines that you work on, as well as the cars you drive more easy!"""
    Answ: Then perhaps a 10mm drill should not exist, instead it should be a 10.05mm drill to make our job easy as well.

    But now I have a question for you regarding unilateral tolerances. If you take the time to research and put in the fit tolerance for a -/- or +/+ dimension, then why the hell can it not be drawn
    to the mean value? Just what makes designers special enough to work out of a standardised catalog and care not about how the "blacksmith" is going to make their design?
    Frankly, I'm amazed that some solids I get can actually be assembled in CAD. If a .5" shaft having a -/- tolerance is drawn to .5 on the nose, and a hole having a +/+ tolerance is also drawn to
    .5 on the nose, then it should not be assemblable in CAD, just as it is not assemblable in real life.

  12. #52
    jim rozen is offline Diamond
    Join Date
    Feb 2004
    Location
    peekskill, NY
    Posts
    21,601

    Default

    "If you use a drill of the proper size as stated, you get holes that will vary from that size to some amount larger."

    Gee. Wonder what would happen if you actually *measured* the sizes of the holes thus produced, and plotted
    their sizes as a distribution. Wonder what that curve would look like. Hmmmm.

    You're over-thinking this thing. If the part calls out for a particular drill size to be used, the manufacturer has
    built that tolerance into the design. Manufacturer has built the stak-on terminal to fit the most likely size
    hole (center of distribution) produced by that drill.

    I'm still waiting for you to explain how the distribution of hole sizes produced by drilling to have a sharp cutoff
    at the low limit, other than simply discarding half the parts.

  13. #53
    Join Date
    Nov 2005
    Location
    Maryland
    Posts
    7,072

    Default

    Quote Originally Posted by jim rozen View Post
    I'm still waiting for you to explain how the distribution of hole sizes produced by drilling to have a sharp cutoff
    at the low limit, other than simply discarding half the parts.
    A drill will not go into a hole smaller than itself. It's one of those laws-of-physics things: "Two objects cannot occupy the same space at the same time."

    In the case under discussion, the two objects are the drill bit and the metal through which it made the hole.
    That's the whole reason a drill bit works in the first place.

    This is the rationale behind plug gauges. If a no-go plug gauge would fit in a hole smaller than it is, it wouldn't do its job, would it?

    I suppose you can find particular situations in which a drilled hole can be smaller. I expect that would happen in some materials due to heating/cooling.
    The parts under discussion are designed for use in metal, generally aluminum or steel. They're not suitable for use with plastics or similar soft materials.

    It has been pointed out that drills can produce larger holes as they wear. This is the reason for the + tolerance on the hole diameter.

    - Leigh

  14. #54
    barbter is offline Stainless
    Join Date
    Oct 2007
    Location
    UK
    Posts
    1,351

    Default

    Quote Originally Posted by benedict leighton View Post
    Well maybe you could step a little back from your point of view one (!) drawing and try to understand the person who designed the whole assembly? !
    Shouldn't need to do this. A drawing is a way of communicating information - nothing to do with psychology


    Most nominal diameters are of round numbers or taken from standardised rows. This was chosen to make designing the machines that you work on, as well as the cars you drive more easy!

    "we'll take this 0,5 inch shaft, fit it in here and then..."

    the shaft will get a -/- or maybe -/0 tolerance because the bushings or the roller bearings are sold as + nothing/ +something.
    I fully understand hole shaft basis, but as I'm getting older, the 'younger generations' (read cad-jockeys) don't seem to.


    Could you immagine how much work it will take for an engineer to recalculate all the round nominals to mean nominals in one complete gear?
    Lazy lazy lazy then. I was always taught that as a draughtsman (ooooh I HATED the term 'designer' ) when detailing a part, work out everything you need to and PUT IT ON THE DRAWING.
    This goes for plating allowances as well as tolerances ie rather than write 0.5 +.0023 / -.0018 for example, write .5023/.4982.
    This was to save anyone else the time of having to EVER work anything out again, and to try to elliminate any mistakes for the life of the part .
    Nowadays there is more and more emphasis on cost down, value for money (read cheap) route cause (and the Spanish inquisition when things go wrong) yet In my experience more and more pictures (drawings I should call them) are produced to a lower and lower standard. And afterall, quality (should) starts in the D.O.


    Now could you brave machinists tell me in a sentence or maybe two what this whole 3 page thread is all about?
    I fit into the less brave - but more foolish category .
    BTW, probably best to never understimate or condescend 'machinists' as there are some very clever ones around here which can do just about everything and anything.
    Last edited by The real Leigh; 06-04-2012 at 03:12 AM. Reason: corrected quote syntax (I think)

  15. #55
    barbter is offline Stainless
    Join Date
    Oct 2007
    Location
    UK
    Posts
    1,351

    Default

    Quote Originally Posted by The real Leigh View Post
    A drill will not go into a hole smaller than itself. It's one of those laws-of-physics things: "Two objects cannot occupy the same space at the same time."

    - Leigh
    Leigh, ever drilled say a 5mm hole into some 0.5mm sheet and seen what you get? The drill will go through (winding in with the flutes), but the hole aint round!

  16. #56
    Join Date
    Nov 2005
    Location
    Maryland
    Posts
    7,072

    Default

    Quote Originally Posted by barbter View Post
    Leigh, ever drilled say a 5mm hole into some 0.5mm sheet and seen what you get? The drill will go through (winding in with the flutes), but the hole aint round!
    1) A twist drill is not the proper tool for putting a hole through thin sheet metal. You should use a punch.

    2) If you run the drill fully through the metal, to the unfluted shank, the hole will be at least the desired diameter, but probably larger and irregular due to damage of the material.

    If you must use a drill in thin sheet metal it should be done using a clamping fixture that holds the work in position and prevents damage, resulting in a proper hole.

    - Leigh

  17. #57
    barbter is offline Stainless
    Join Date
    Oct 2007
    Location
    UK
    Posts
    1,351

    Default

    Quote Originally Posted by The real Leigh View Post
    1) A twist drill is not the proper tool for putting a hole through thin sheet metal. You should use a punch.

    2) If you run the drill fully through the metal, to the unfluted shank, the hole will be at least the desired diameter, but probably larger and irregular due to damage of the material.

    If you must use a drill in thin sheet metal it should be done using a clamping fixture that holds the work in position and prevents damage, resulting in a proper hole.

    - Leigh
    Leigh - see that smiley face there i'm playing with you. I remember drilling this back when I was an apprentice and couldn't understand how the drill had gone through but not produced the drill size hole

  18. #58
    Join Date
    Nov 2005
    Location
    Maryland
    Posts
    7,072

    Default

    Quote Originally Posted by barbter View Post
    Leigh - see that smiley face there i'm playing with you.
    Yeah, I know. No problem.

    Sometimes my responses are really for the benefit of readers who pull these threads out of the archives, and not directed to the immediate respondent.

    I too have screwed up more pieces of sheet metal than I care to admit.

    - Leigh

  19. #59
    Glenn Wegman is offline Stainless
    Join Date
    Jan 2007
    Location
    Florida
    Posts
    1,014

    Default

    Kind of off topic, but since drills entered into it...

    Try using a double margin drill.

    Much better and nearly round hole in sheet metal, as it eliminates the tri-lobe effect.

  20. #60
    Join Date
    Nov 2005
    Location
    Maryland
    Posts
    7,072

    Default

    Hi Glenn,

    What is a "double margin" drill?

    I use step drills for most holes in thin metal and they come out perfect every time. Great invention.

    - Leigh

Page 3 of 7 FirstFirst 12345 ... LastLast

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
  •