yang686526

gd&t machined octagon centered on shaft
lets see if you guys can figure this one out,
i'm correcting old designs and drawings for my company, and i'm trying to clearly indicate the concentricity of an octagon shape on a shaft.
this octagon is to be press fit into a pinion (68mm h6).
datum [a] is the center of the shaft.
the ground cylinders that will mate with bearings are: '[con|Ø0.030|a]'.
i've looked at using basic dimensions: [3x45.00°] & [sym|0.000(m)|a] except that symetry does not allow the of mmc.
do i have to use profile tolerance for this application?
"concentricity is is a condition of a surface of revolution in which all points of the surface are equidistant from a common axis."
an octogon does not meet these conditions. profile may be the best alternative.
the application of concentricity is complex and rare. i would consider uses position, runout or profile before concentricity but in your case i would use profile.
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
_`\(,_
(_)/ (_)
never argue with an idiot. they'll bring you down to their level and beat you with experience every time.
i agree with heckler. i very rarely used concentricity. it is more difficult to inspect.
chris
systems analyst, i.s.
solidworks 06 4.1/pdmworks 06
autocad 06
amen to profile. it is the way to go for this application.
my preference would also be to use profile of a surface. there is another alternative, however.
you can use positional tolerace to locate the center plane of opposing faces because they are features-of-size. this also allows you to use mmc if appropriate.
jim sykes, p.eng, gdtp-s
profile services
cad-documentation-gd&t-product development
i as well agreewith heckler. i would go get the octogonal material from stock, check central steel and wire catalog. this is a stock item.
regards,
namdac
getting closer?
cylindricty and the 2 runouts are applicable on round features of size - not applicable here.
the profile of a surface is theoretically applicable since it would control the shape and location relative to the datum but one must have a cmm with scan mode to measure this feature. it would not be measured on the shop floor well unless this equipment is available.
positonal tolerances may be the best approach and one could use mmc. i would suggest a 0 tolerance beyond mmc since this hex shape has a snug assembly fit. i would also reference my datum(od) at mmc. i might even place the word "boundary" below this fcf. the virtual condition is actual the mmc size and shape of the hex.
this would then be conducive to a checking fixture in which there would be a hole of mmc size for the datum and hex at the mmc size and in true position to the datum. one would then place the part datum first into the fixture and rotate the part so that the hex lines up. the part should then be able to be pushed (with the force of 1 finger) all the way down in the fixture. if it goes all the way, presto, the feature is within tolerances.
this feature could then be confirmed on the shop floor by the operator.
dave d.
mechtech, getting there, but not done yet. pls click on the following link for how i'd tackle this, at least at first glance.
mechtech2000,
i looked at your drawing.
if your octagon is being pressed into a mating octagon shape, your tolerancing should be very simple, albeit, very accurate. just use a profile tolerance all around. the symmetry and the +/- tolerances do not help you. your drawing defines the distance between opposite faces very accurately, but allows adjacent faces very much more error.
if it were my drawing, the surface tolerance would be 0.01 all around, and i would use a phantom line to show that this error all went inside from nominal. see figure 6-15 in asme y14.5m-1994. i would not bother with the point to point dimension except maybe as a reference. i would specify the radius sloppily as something like +0.5/-0.
jhg