【转帖】location information for hole position relative to basics

yang686526

location information for hole position relative to basics
i was given a drawing by my design to review and forward to a supplier. i will describe a simple version of the part.  consider a bar with three holes in them.  the face of the bar is datum a.  the center lines of holes 1 and 2, most important holes, are datums b and c.  hole 3 is also important and the center line of that hole is (0,0).  
now the question, there are no basic dimensions on the drawing because the drawing is to be associated to the 3-d body provided with the drawing.  there are true position call-outs for all three holes relative to datume a,b&c.  my customer is requesting data on not only the true positions but the locations of the centers of these holes as well.
i can have the basic dimensions added.  i also plan on having the datums changes so that the true positions are not relative to themselves.  how do i dimension the drawing so that the supplier knows to measure and provide data for both true positions and location of the hole centers?
are you calling these holes to be drilled on assembly? or will they stand independent to the part they pass through?
this is my take on this but without being privy to the design it's just a blind guess.  datum -a- is good but make the first hole datum -b- then reference the other two holes to datum -b-.  because you made all the holes datums you have created what excel calls a circular reference....with no other features to reference to.
a circular reference is created when a formula refers back to its own cell, either directly or indirectly.
best regards,
heckler
sr. mechanical engineer
sw2005 sp 5.0 & pro/e 2001
dell precision 370
p4 3.6 ghz, 1gb ram
xp pro sp2.0
nvidia quadro fx 1400
      o
  _`\(,_
(_)/ (_)
"coming together is a beginning, staying together is progress, and working together is success." - henry ford

i agree with heckler.  it's very confusing to try to hold datum b positional to datum b (and c to c).  if you have a good straight edge, you could define that as datum b, and the first hole as datum c.  hold the other two holes positional relative to a, c & b.  you then have more control over the orientation of the common center line between the holes.
thanks for the replies.  this is a plastic molded part.   this part, along with a mirror of this part use these holes align mating components (rods) between them.  just to be clear, only two holes are datums. this was done for measurement purposes.
my remaining question; is there a way to dimension these hole locations such that i get the true position data as well as the locations in x and y relative to hole, (0,0)?  my understanding is that basic dimensions, required for true position, are inherently not measured not reported.
this is not so.  basic dimensions are measured, and are toleranced according to the feature control block.
on a molded part, however, you may get by with only measuring the first couple of parts produced, to verify the mold and process.  after that, fewer features need to be inspected to insure part conformity.
as to having two holes being datums, this is ok, as long as you don't have a circular argument as heckler pointed out.  you can't position datum b relative to datum b, etc.
terbo29,
   i consider that using the holes as datums is reasonable.  your inspection fixture is a flat plate with a round pin and a diamond pin corresponding to holes a and b.  if your positional tolerance is with respect to three datums, than it is implied that only one datum applies to hole_a, and two datums apply to hole_b.
   you _can_ inspect hole b, but only in one direction.  effectively, your positional tolerance becomes a +/- tolerance.
   presumably, the outline of your bar is much less important than the holes.  probably, you should apply a profile tolerance to the outline.
   if this assumption is true, you have an alternate dimensioning strategy.  you can use the side and one end as datums b and c, and dimension your holes from these. apply a composite positional tolerances as shown on figure 5-19 of asme y14.5m-1994.  
   yet another alternative is to use the width and length as datums, and specify these at mmc.
   i have problems with your concept of "true position".  there are two obvious ways to dimension your bar, especially assuming your holes are symmetrical.
1. dimension the thickness, width and length of the bar, and dimension between the holes.  as per asme y14.5m-1994, if it looks symmetrical, it is symmetrical, and true position is based on that symmetry.  it helps show that your design intent was symmetry.
2. dimension everything from one side and one end.  your true position is called out explicitly.  it makes sense to use the side and end as datums b and c.  this is probably good practise if your bar is not symmetric.
   the best thing you can do is ask yourself how your inspection fixture is going to work.  if you are fixturing this thing over a pair of pins, your datums should be two holes.  if your datums are edges or the width, your fixture should pick these up.
   if you are using +/- tolerances to locate holes, the dimensions _must_ come from the critical features.  with positional tolerances and basic dimensions, this is not absolutely necessary, although it is still good practise.  geometric tolerances explicitly define the datums used to locate your features.  
                            jhg