yang686526

positional tolerance query
hello, i am new to this site. i am seeking advice on the proper method of considering a specific positional tolerance feature on an aerospace drawing that i am working with.
the specifics are 200.600 a bolt circle that is basic for diameter and hole spacing, toleranced by a feature control frame as follows: true position symbol/.030 dia. positional tolerance of holes @ mmc /datum a /datum c @ mmc.
the holes are toleranced: .404-.413 thru holes on a flange.
datum a is the flange face, datum c is the outside diameter of a cylinder that is concentric with the bolt circle but on a different plane. datum c's diameter is toleranced 198.950 +.060/-.030.
my problem is the bolt circle diameter of a particular part in production is small (-.035" from basic, -.0175 for each hole from their true position in "x"). the holes are otherwise spaced / clocked correctly. i consider the positional deviation to be at least .035 plus any datum deviation. i instructed that the holes be opened up to .411 in order to utilize bonus tolerancing from mmc and i now feel that the bolt circle meets print. (i hope that i am interpreting this situation correctly).
as an added concern, i have been told that i did not need to open up the holes because i could use additional bonus tolerancing (shift tolerance?)for datum c's deviation from mmc. this diameter is inspected at:198.982 (.028 from mmc).
is it correct to also use this bonus tolerance? do you consider half of its value? i informed all that i did not agree with this interpretation but some in engineering and management are against me on this.
the customer rep is siding with me but i could sure use some advice on the proper way to interpret this situation.
the customer print refers to ansi y14.5m-1982.
thank you for you time and advice.
find a job or post a job opening
the virtual condition of your 'specifics' bolt pattern is .374 diameter (.404-.03)(mmc-geotol).
a gage with a diameter 199.01(mmc) opening and pins of .374 spaced as instructed on the 200.6 bolt circle would validate the condition described. as your physical datum c deviated from mmc, it would permit the part to shift on the gage to confirm if the .374 pins would simultaneously go thru all the bolt holes.
hope this helps.
thank you for your reply. i follow your explanation of the "virtual condition" for the holes. i believe that i was considering this in an accurate manner by considering my initial tolerance in "x" of .030 / r .015. i also think it is permissable to use the bonus tolerancing of .007 / r .0035 since the holes are .007 from mmc.
unfortunately, this inspection is primarily done mechanically, being too big for our cmm or for a gage. initially, the hole pattern is verified with a co-axial indicator on the machining center but for diameter inspections this is not possible for a few reasons.
as far as considering the secondary datum's "shift tolerance", i was reluctant to incorporate this, as the customer opened up the tolerance on this feature from
+/- .015 initially to +.060/-.030! i do not know if they considered how this would effect the bolt circle toleraning.
based on your explanation, would the statement be accurate that i could consider another .014 shift tolerance per hole, (.028 on diameter?), since the datum diameter mover .028 from mmc?
this would certainly provide a huge increase in available tolerance, (of which possibly the customer did not intend).
also this would coraborate what others at our shop had stated.
again, thank you for your help.
a diameter of 199.010 would permit 0 shift.
a diameter of 198.920 permits 0.090 shift.
199.010 (mmc of datum c) - xxx.xxx (actual measurement) will give you your shift value.
the shift variation was increased by .060 (.090(current)-.030(previous)).
thank you again for your explanation and assistance. i understand this matter more clearly now.