【转帖】best method

yang686526

best method?
i have question pertaining to machining 2 cast boxes and then assembling them.  on our machining prints we usually reference the outside cast features of our cast boxes as a datum, and then reference the mounting holes (tapped holes on one part and screw clearance thru holes on the mating part) to be within say .020 true position of the outside feature.  this essentially lets manufacturing know that whatever the outside dimension of the cast part, the mounting holes are to be centered within .020 of that overall length/width.  this is understood here by both engineering and manufacturing.  manufacturing will add a few lines in the program to have our machines probe the outer features of the part during machining in order to determine the hole locations.  what this does for us is average out the sand casting variations so that we get a best alignment of the two cast boxes when assembled.  i have been looking for this method in either lowell/foster geometric tolerancing book or the ansi y 14.5 book to see if this is a generally accepted, but have been unable to really find anything significant.  is this method generally accepted/defined?  does anyone have a method that works best for them? i now have a case where the mounting holes are not equally spaced from their respective edges of the casting (the mounting hole pattern is not centered in the cast box by intentional design) and was wondering what solutions are used in your respective company to best align parts in this situation to prevent there from being some ugly cosmetic appearance of the parts shifted to one another due to casting variations?  i hope i have explained my situation clearly.  thanks in advance for any help you can offer.
pete yodis
find a job or post a job opening
establish the datums as being the center of the length and/or width of your cast box and then the holes are positioned in relation to the established datums. your true position of .02 will still work. you could go to a composite tolerance, where the pattern of holes in relation to each other is a tighter tolerane than the whole pattern is to the established datums.
there is nothing that says the holes must be equally spaced, except the method you have used to dimension them from the datums.
to define a datum across the outside of a box, put the datum symbol below the dimension that measures across the outside of the box. this will establish the datum as being the center plane between the outside faces of the box.
"wildfires are dangerous, hard to control, and economically catastrophic."
"fixed in the next release" should replace "product first" as the ptc slogan.
ben loosli
cad/cam system analyst
ingersoll-rand
ben,
   thanks for the reply.  is this defined in ansi y14.5?  are you saying that you can place a centerline in the drawing through the theoretical middle of the length and width of the part as defined by the overall datums, and then dimension any of the holes from that centerline?
to clarify ben's post...
the methodology is correct, but be sure to label the dimensions as the datums, and not the center planes.  the features are the datums; the geometric controls will be relative to the datum center planes.  these planes are not datums in and of themselves, but relate back to the features.
is it accepted practice then to dimension holes from the center planes as established by the datums?  would you annotate your drawing to show a center plane and then dimension from that?  would the center plane appear as centerlines on your drawing?
yes, you can dimension from the center planes, and they would appear as center lines (as long as they are normal to the view).  just don't label those center lines as datums.  if you do need to label them, prefix the datum callout with "center plane" or something similar.  y14.5 states in para 4.3.2 "the datum feature symbol identifies physical features and shall not be applied to center lines, center planes, or axes..."
ben and ewh,
   thanks for your help.
pete yodis
just to clarify,
it is asme y14.5m-1994, not "ansi".
chris
sr. mechanical designer, cad
solidworks 05 sp2.0 / pdmworks 05
first, the casting drawing should have cast datums and datum targets defined.  then usually casting houses like to apply a general surface profile to those datums.  then the machined drawing should have a completely seperate datum structure that is tied back to the cast datum targets/planes.  then all your machined features should be referenced from machined datums.  locating features from an imaginary center line or axes imho can create ambiguity.
best regards,
heckler
sr. mechanical engineer
sw2005 sp 2.0 & pro/e 2001
dell precision 370
p4 3.6 ghz, 1gb ram
xp pro sp2.0
nivida quadro fx 1400
      o
  _`\(,_
(_)/ (_)
do you trust your intuition or go with the flow?
hi guys,
just a quickie related to fasteners. would anyone tell me what ifi 513 standard is?
thanks in advance.
fevfdl
pdybeck-
there is an asme standard specifically for the dimensioning and tolerancing of castings and forgings.  that standard describes equalizing datums that are designed to establish datums on centerplanes using a symmetrical array of datum targets.  i don't know the number but i'm sure it is referenced in asme y14.5m-1994.
note also that width datums can be used.  this kind of datum is associated with(and attached to) the dimension of any feature of size formed by two parallel, opposing surfaces.  this may be an inside dimension or an outside dimension.  in this scheme, the datum reference plane falls on the centerplane of that width (or length of whatever you choose to call it).  the hole locations then originate from the centerplane(s) which makes their locations completely independant of the part size!  for each centerplane the machinist establishes datums on each of the two opposing surfaces then divides by two.  he then establishes an orgin there.  note that width datums can generate additional bonus tolerances because they are based on a feature of size.
tunalover