【转帖】position tol of tapped hole

yang686526

position tol of tapped hole
i have a tapped hole on the end of a precision shaft. the hole is on the center line.  what is the best way to apply a postion tolerance so that the threaded hole stays on the centerline?  the shop that makes the part seems to have a hard time with keeping the tap straight and i want to make sure that the drawing is providing enough information to them.  thanks.
check out our whitepaper library.
matalik,
   are they having a hard time locating it in the centre, or is it crooked?
   a true position tolerance tells the fabricator how to locate your hole.  true position controls parallism to the od and/or perpendularity to the end face, but not very accurately.  you can use a parallel or perpendularity specification, in addition.
   perhaps it is time for a new machine shop?
                  jhg
you can put all the controls on the drawing but unless the manufacuturing engineer has the process/fixture for that feature contrained you will end up with a "bad part"
best regards,
heckler
sr. mechanical engineer
swx 2007 sp 2.0 & pro/e 2001
dell precision 370
p4 3.6 ghz, 1gb ram
xp pro sp2.0
nvidia quadro fx 1400
      o
  _`\(,_
(_)/ (_)
(in reference to david beckham) "he can't kick with his left foot, he can't tackle, he can't head the ball and he doesn't score many goals. apart from that, he'
the first question you need to ask is 'how accurate does the hole need to be' then look at how to tolerance it to meet this requirement.
looking at the use of gd&t as a quick fix without understanding how accurate the feature needs to be causes problems.  gd&t should be driven by functional requirements.
once you've determined what accuracy, you need then look at if just positional to the end face & od is enough or do you need extra controls to keep it 'concentric' (note that i'm not actually suggesting to use concentricity tolerance)
drawoh
quote:
true position controls parallism to the od and/or perpendularity to the end face, but not very accurately.
surely how accurately depends on what value you assign to the tolerance?  
matalik,
(kenat, good advice)
gd&t will not 'solve' this problem, it will only emphasise what is required by you (the engineer) to your manufacturer (assuming he can understand what you send him).
i would suggest one of the following...
1. get your manufacturer to pilot bore the shaft to one amd quarter times the full thread depth (gd&t this bore perp and par to shaft centre axis). then gd&t tapped hole to bore (conc)
2. reject all inferior material back to your manufacturer. may lead to arguments, so make sure your dims (and gd&t's) are correct.
3. get a new manufacturer, and before you change to him, make sure your prod/manufacturing engineering audit him to make sure he can do what you require.
kevin hammond
mechanical design engineer
derbyshire, uk

thanks, i have my answer.  the shop is having a hard time keeping the tap straight, so if i gd&t the hole to the axis, then gd&t the tap to the hole as suggested, i should be covered.
i don't think i've ever toleranced the bore and thread separately before.  i dont' have access to the standards today but i'll have to look at it when i do.
also, wouldn't it be better to use a physical datum rather than the theoretical axis?  or are you going to effectively define the axis by making one end a and one b and having the bore reference a-b or something?
if it's a shaft, is parallel really the right tolerance, if positional isn't adequate would runout be better given that you appear to be concerned about 'concentricity'.
i'm getting in above my head now, you know what they say about a little knowledge, sorry.  maybe one of the more experienced posters can comment.
plus when i said function should drive the tolerancing, obviously you still need to verify that what you think you need can be physically achieved, it just shouldn't be the initial driving factor.
kenat,
   i routinely apply true position tolerances of 0.2mm on drawings.  this is accurate enough to locate tapped holes and clearance holes for machine screws, assuming the clearance holes are through thin material.
   if the tapped hole is 10mm deep, the fabricator can use up his entire error budget by angling the hole 0.2mm.
   0.2mm/10mm = .02 radians.
   this is over a degree of error.  if you stick a long screw in it, you will see this clearly.  if the clearance hole goes through thick material, the screw will not clear, and you will have a non-functioning assembly.
   i have seen this done.  you can drive a tap crookedly into a good perpendicular hole.  it helps to do it when the forman is not watching.  
   if you have a deep clearance hole, you should consider adding a perpendularity specification to your tapped hole tolerance.  i haven't actually checked this, but my gut feeling is that perpendularity of 0.05mm should be manageable by a machinist with a hand tap.  machinists, please feel free to correct me.
                         jhg
   
   
thanks for the additional thought.  that's what i am getting confused about.  i have been trying to look at examples and don't see one where they gd&t the bore and thread separately.  
it seems like there are several ways to do this, so i'll take any other thoughts.  i'm looking for expamples of a similar situation, but am having a hard time finding any that have threaded holes.
initially (i didn't create the part), the bore and thread are called out on the centerline of the shaft with no gd&t.  i have limited experience in this area, and when parts started to fail, i have to clean up the mess.  i guess its a good time to learn.
what i am seeing in examples, they gd&t using position first then perp, so that the bore will be in the correct position and square to the face of the part.
matalik,
   when you say "bore", are you talking about the tap drill?
   as the designer, drafter and inspector, you have no interest whatsoever in the tap drill.  don't specify it.  don't apply tolerances to it.  don't inspect it.
   machinists know, probably much better than you do, what size drill to use prior to tapping.  if your machinists need you to tell them this, this might be the source of your problem.
   for a tapped hole, specify the size, the pitch or tpi, the tolerance class, the depth, and the positional tolerance.  add a perpedularity specification to the tolerance box if you need it.  buy thread gauges to inspect it.
   if your bore has some functionality other than allowing you to tap a hole, then you apply the tolerances needed to meet that functionality.
                   jhg
i would place a positional tolerance on the threaded hole relative to the axis created by the od.
this would be fine at the end surface but it still does not control parallelism.
since this is a blind hole, i would also place a projected tolerance of at least the depth of the hole in the feature control frame.
how to check this - there would be a small checking fixture that threads all the way down in the hole. protruding up from the hole on this checking fixture would be a cylindrical shaft the length would be the projected tolerance length.
once installed in the threaded hole, check the position at the end face of the shaft and also at the end of the checking fixture cylinder which controls the parallelism.
that should do it.
dave d.