Best method?
Best method?
(OP)
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
Pete Yodis





RE: Best method?
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
RE: Best method?
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?
RE: Best method?
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.
RE: Best method?
RE: Best method?
RE: Best method?
Thanks for your help.
Pete Yodis
RE: Best method?
it is ASME Y14.5M-1994, not "ANSI".
Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP2.0 / PDMWorks 05
ctopher's home site
FAQ371-376
FAQ559-1100
FAQ559-1091
FAQ559-716
RE: Best method?
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?
RE: Best method?
Just a quickie related to fasteners. Would anyone tell me what IFI 513 Standard is?
Thanks in advance.
FEVFDL
RE: Best method?
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
RE: Best method?
Thanks for the repsonse. This is in fact how we dimension our machined enclosures here (see my first post). I was checking to see if this was a generally accepted practice and/or one that was defined explicitly in a specification somewhere. I was not sure if it was just something which was understood or utilized at my company, but from the response it seems to be the norm. Would you be able to find the ASME standard number for dimensioning and tolerancing of castings?
Pete
RE: Best method?
It is ASME Y14.8M - 1996 Castings and Forgings (which took all of two minutes on the ASME website to determine).
Tunalover
RE: Best method?