【转帖】calculating positional tolerance

yang686526

calculating positional tolerance
i am familiar with using the x,y tolerance range to calculate a diametrical positional tolerance (the square with a circumscribed circle method) using the sqrt(x^2+y^2) equation.
i have a very simple drawing of a plate with a bunch of holes through it and all dimensions are +-.01. i need to apply gd&t to the drawing. is it correct to simply use the above method to calculate all the positional tolerances? (in which case the tolerance would be the same for every hole since all dimensions are +-.01) it seems too easy.
i have no knowledge of the pin/shaft to go through the holes, or if it's a hole on another plate to be alligned. is this information needed to apply a positional tolerance to the hole?

there is a difference between calculating equivalent positional tolerance for +- tolerance and applying the correct tolerance.
your equation will get you the equivalent positional tolerance, .028".
to get the correct tolerance (ensure fit/function) yes you need the mating part information and to use the equation stated in appendix b4 of asme y14.5 (also in my spreadsheet on
just realized, i'd assumed it was a fixed fastener situation, if not then the floating fastener calc should be applied.
kenat,
jlang17
you need to times 2 ( x2 ) on your equation above to get the correct data.
there are two simple ways to get the positional tolerance :
1. positional tolerance = overall plus / minus tolerance x 1.4142
example : ±.01 = overall .02 tolerance
positional tolerance ? = .02 x 1.4142 = .0283
overall plus/minus tolerance = positional tolerance ? x .70711
example : positional tolerance ?.0283
overall ± tolerance = .0283 x .70711 = .020 overall = ±.010
2. if you don't like calculation, you may convert it from the chart ( as attached )
hope this will help you
seasonlee

whether the op needs to x2 depends on if they enter the total tol range or the deviation from mean, they don't explicitly state which they are using.
kenat,
jlang17,
   the positional tolerance equivalent to ±.01" x/y tolerances is ?.028".  this is all assuming that your x/y tolerance was intended to allow a hole to be .014" out of position.  it is always possible that the designer was trying to do something else.  
   a convenient estimate is that a clearance hole for a bolt requires a positional tolerance equal to the hole clearance, c=drill-screw.  for a screw in a tapped hole, the geometric tolerances should be c/2.  
   note that drilled holes are oversized and screw major diameters are undersized.  i call up my clearance holes as +tol/-0.  in the case of the screw, it is assumed that the material being clamped is thin.  otherwise, you must account for the perpendicularity of a screw in an angled hole.  also, it is assumed that both parts are being made to the same tolerance.  if you are clamping a casting with cast-in holes, to a machined mount, you may want to mess with the model a bit.
               jhg
i know some people don't like the formatting etc. but take a look at the spreadsheet.  it uses the terms/formula from 14.5 which is basically the formula drawoh gives.  the tab 'example 3' may be especially useful.
all this calculating is fine, but the whole point of true position gd&t is to buy off the parts that would normally fall outside the square tolerance and within the circular tolerance. additionally, it allows for easier calculation of mating holes and "bonus tolerance."
so, if the problem is just converting cartesian tolerances to diametral tolerances, i'd say use the chart. if the object is to re-engineer the parts to maximize the gd&t, then you probably want to fire up the calculator. but even in that situation, i tend to stick to standard tolerances (?.014, ?.028, ?.042, etc.) and i tend make the holes the nearest drill size up, instead of the exact hole size (unless you need the exact hole size, of course).
wgchere, it's to buy off parts that fall outside of the square so long as they work.  typically when i see nice round numbers such as +-.005 or +-.010 it's because people have invoked block tolerance.  this for hole patterns usually means they haven't correctly considered tolerancing.  so i stand by my distinction between equivalent and 'correct'.
i agree with choosing standard drill sizes whenever possible, along with typical drill tolerances but never understood the obsession with 'standard' position tolerances.  i always use the largest that the fastener/drill/function will allow.
kenat,
thanks for the responses. now i have another question, which i'll try to explain the best i can.
i have tapped holes called out for #6-32. most charts will tell you the screw size is 0.138 and the tapped hole size is 0.1065. once the hole is tapped, it is increased to 0.138. so now the screw size and hole size are the same. if i want to position at mmc (let's say +-.005), i'm left with a negative tolerance since the screw is increased to 0.143 and the hole is decreased to 0.133.
or do i consider the chart to be at mmc? so it would read screw size 0.133 (+-.005). and hole size 0.143 (+-.005). this then would work fine, but i don't know if these charts are suppose to be read at mmc.
jlang17, i always use the screw max dia for my calculations.  you don't need to worry about what the tap size is, you need to worry about what the clearance hole size in the mating part is.
i think you may be totally confused.  the chart seasonlee posted is just for converting +- dimensions to equivalent positional diameter.  it isn't for calculating the required tolerance to ensure fit.
use instead the equation drawoh gives which is the same as in my excel sheet.  take a look at the examples in my excel sheet hopefully they'll help you.
simplistically for fixed fastener:
1. subtract the screw max major dia from the minimum hole diameter.  
2. divide the result between the threaded & clearance hole.
it's often better to give slightly more of the position tolerance to the threaded hole as it doesn's benefit from mmc and with 2 operations (drilling & tapping) generally has more tolerance accumulation.
if you're still confused post the clearance hole diameter & it's tolerance and i'll try to find time to do a worked example for you.
kenat,