GD & T Thru hole callout
GD & T Thru hole callout
(OP)
I have a part I am working on that is .250 thk aluminum. The problem I have is that when I pierce the hole I am out of the general tolerance on the bottom due to the blowout. My customer wants to reject this, The print is interpreted using Y14.5M-82. How would this be stated on a print that the hole size must be in tolerance all the way thru or is it assumed that the holesize must stay within the general tolerance block.
Talk To Other Members
RE: GD & T Thru hole callout
It is understood in the stamping industry the the hole is measured at the cut and not the break. One can control the cut with your pin but the break is not controllable. If your Customer wants control all the way through, then I would suggest that the hole be drilled at a greater cost.
I have dealt with quite a few automotive stamping companies and have seen Designers take off a drawing profile of a surface since the break could not be controlled. They have replaced it with profile of a line.
Hole this helps.
Dave D.
www.qmsi.ca
RE: GD & T Thru hole callout
Rule #1 (the Feature of Size Rule) of ASME Y14.5M-1994 (and ANSI Y14.5M-1982) states that that a feature of size such as a hole establishes a boundary of perfect form at MMC. If the hole is produced at MMC (minimum diameter) then it must be of perfect form. Variations in form are permitted as the hole size departs from MMC (as the hole gets larger).
Secondly ASME Y14.5M-1994 (and ANSI Y14.5M-1982) states that UNLESS OTHERWISE SPECIFIED, THE TOLERANCES APPLY TO THE FULL EXTENT OF THE FEATURE. In this case all tolerances (the size tolerance and any positional tolerance) apply over the depth of the hole (which of course is the same as the plate thickness for thru-holes). If the hole diameter is out-of-spec anywhere through the thickness then it doesn't meet the drawing.
If the drawing calls out a nominal diameter without explicit size tolerances (shown next to it in the field of the drawing) then the block tolerance usually applies by default.
If you have a block tolerance .XXX: +/-.005 and the hole is called out as .141 DIA then the hole boundary must reside within a hollow cylindrical zone that has an ID of .136, an OD of .146, and a length equal to the plate thickness. If a plug gage that is bigger than .146 can fit in the flared end of the hole then the hole is out-of-spec.
Am I kicking a dead horse yet?
Tunalover
RE: GD & T Thru hole callout
You are absolutely theoretically correct about the ASME standard. It does state size for full depth. You are correct.
The Customer does have a claim that cannot be met using a stamping operation. Drilling - absolutely. Stampings can only control the cut and not the break.
People need more design reviews out there and these situations should be noted. The drawing could have stated that all dimensions are controlled at the cut side.
As far as a dead horse, no way. GD & T is not easy. I have been in the quality game for so many years and GD & T for about 20.
There are soooo many questions and situation concerning GD & T out there on the shop floor. We need more clarification in the standard or on the drawing.
Dave D.
www.qmsi.ca