yang686526

can symmetry be implied without gd&t?
a part has a defined center line, features are symmetrical about that center line. distance between the symmetrical features (tapped holes) is important. is a dimension mandatory from the center line to a feature on one side?
or is it allowable to leave that dimension out to imply symmetry and not a tolerance stack to one side of the center line?
it's been common for many years to just dimension between the two points and put "= =" under the dimension line (i believe there was a thread on this a while back). it's not part of any current standard that i've heard of, so it may not be recognized by the shop. a second consideration is that a centerline doesn't exist on a physical part, so how are you going to check those positions without defining that centerline, which essentially is the domain of gd&t.
in other words ... do the gd&t!
jim sykes, p.eng, gdtp-s
profile services
cad-documentation-gd&t-product development
the centerline is extended from a hole in the center of the part so there is an actual feature to use as a datum. trouble is they frown on the use of gd&t unless absolutely necessary here. otherwise i'd use it.
cwdaniel,
if your part looks symmetrical and the drawing is specified as being done to asme y14.5m-1994, then symmetry is implied. this is true, gd&t or no gd&t.
without asme y14.5m-1994, there is no standard to interpret your drawing by, and you should make things explicit.
jhg
if you are concerned about reducing dimensions on a symmetrical part, you can place a centerline on the part with "=" at each end as shown in asme y14.2m-1992 (referenced by asme y14.5m-1994). this is just a visual way of saying that the dimensions and tolerances apply idenically and individually to both sides of the part. you will want to verify that your tolerance stack ups are still valid if you do this. the better method is to, in jim's words, "...do the gd&t!".
david
keep in mind that there is a difference between dimensioning (the goal) and tolerancing (how much you can blow it by). with dimensioning, a symmetrical relationship my be implied. but, features shown symmetrical must be controlled with geometric tolerances according to y14.5. in other words, listen to jim. by the way, gd&t doesn't make parts expensive--tight tolerances do.
ditto!
what the others wrote.
chris
solidworks 06 4.1/pdmworks 06
autocad 06
cwdaniel
quote:
the centerline is extended from a hole in the center of the part so there is an actual feature to use as a datum.
some of the above are sharper on gd&t than i but to me if you don't use it then you haven't really told them to use the hole as the datum. they may be just as valid using the outside dimensions or some other symmetrical feature.
i've seen implied symmetry cause problems before so i'd always make it explicit.
quote:
by the way, gd&t doesn't make parts expensive--tight tolerances do.
if only we could convince everyone of this!
kenat,
you are right. the datum must be called up explicitly on the drawing. it can be the hole. it can be the two outside edges. in either case, your datum is a feature of size. unless it is very accurate, you should call it up at mmc. this may be an issue with the functionality of the part.
i have an issue with the idea that gd&t is somehow more complicated and expensive than no gd&t. a recommended procedure on a part like this is to apply a composite positional tolerance. one true position attaches the pattern to the face sloppily. the other true position locates the holes accurately with respect to each other. this is an ideal solution when you have to match the holes in the mating part, but you are not concerned about the overall location.
in effect, the symmetry is nominal, not actual.
i am not sure what happens when you do not apply basic dimensions. the asme standard goes very quickly into positional tolerances and true position. i would regard non-basic dimensions as ambiguous.
jhg
all that making a dimension basic does is tell the person reading the print that that dimension does not follow the standard tolerences set up in the tolerance block and that the tolerance to apply is shown elsewhere. it tells them to assume the dimension to be theoretially perfect.
david
aardvarkdw,
i am assume that when you do not make the dimension basic, you also do not apply the positional tolerance.
let's assume our part is a rectangular plate, let's continue to interpret the drawing through asme y14.5m-1994, and let's assume the tolerrance block in millimeters says x=+/-0.5, x.x=+-0.2 x.xx=+/-0.1, and angles are +/-1deg.
the sides of the plate are allowed be one degree out of perpendicular to the base. are orthogonally dimensioned holes measured from the angled side, or from the corner at the base?
if both sides are one degree out of perpendicular in the same direction, how do you determine where symmetry applies?
if you ask yourselves these questions, the gd&t positional tolerance becomes simple.
jhg