positional tolerance query

[riverdave]

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.

 

[weavedreamer]

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.

 

[riverdave]

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.

 

[weavedreamer]

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)).

 

[riverdave]

Thank you again for your explanation and assistance. I understand this matter more clearly now.