I don't think that is a valid callout. I don't have ISO 2768 handy but in ASME Y14.5, perpendicularity has to be applied to a surface or a feature of size.
The print is ISO standard, the standard of ISO 2768 is a general tolerances for linear measures,its better to revise my post to : the tolerance standard is ISO 2768.
There are versions of the ISO standards that certainly would allow that, in my opinion, The callout you are looking at is more likely covered under ISO 1101. My understanding is that the newer ISO versions will not recommend the practice of references directly to centerlines. I am not an inspector so I can not you help you alot on specifics there.
Frank
If an explicit tolerance is called out on the drawing that takes precedent over the general iso2768 tolerance as I recall. ISO 1101 may be correct, I can't recall for sure.
Its ISO 1101. I checked in a old copy (1983 Edition).
They Show Datums and features to centerline. Also it mentioned if datum precedence is not Important Both datum Names A & B can be Given in Same Box !
NX 6.0.2.8 MP4
Teamcenter 2007
WINDOWS XP (64 Bit)
FYI -- that was tossed out in the 2004 edition of ISO 1101. (If you have that version, see the appendix, paragraph A.4.) Now ISO requires the datums to be given in a specific order, just as ASME does. That makes sense; to have no precedence among the datums as allowed by the 1983 edition was either a) implying that the datum features would always be perfect, or b) ambiguous, which defeats the very purpose of GD&T.
John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
I dont have ISO 1101 (2004).
But atleast now i am aware that ISO and ASME are almost similer.
Is there any PDF or Document which shows the differnce between ISO 1101 (2004) and ASME y14.5 M 1994 .
Thanks in advance.
*Problem is in our Organization many dwgs are based on old ISO standards.Now we are Updated it to ASME Y14.5 (1994).
But lot of confusion with people regarding the Symbol and representation of GD&T .
Initially i Thought most of old dwgs are wrong regarding GD&T. But recently i got hold of this old ISO PDF then realised dwgs are alright , i am Wrong
NX 6.0.2.8 MP4
Teamcenter 2007
WINDOWS XP (64 Bit)
I thought the same, until I pulled out the ISO standard. The 1983 version explicitly says that "AB" means that the "sequence of two or more datums is not important." There is a separate blurb explaining the different "A-B" as a common or combined datum.
This was even more confusing because ASME allows "AB" if all single letters of the alphabet are exhausted (other than I,O,Q). But apparently the old ISO standard didn't have any provision for identifying datums beyond single letters. Shrug.
John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
J-P,
Agreed, I see that they have both in '83 as you've stated. I suspect that it was a case of oversimplification and someone realized that on a large part theoretically they may actually reach datum "AB". Naturally the choice of actual datums "A" & "B" will have an effect on that what was intended if they were two concentric features on a shaft/boreline I suspect it was the same thing, probably to carry over from a earlier practice.
I believe I have seen engine blocks with an awful lot of datums; I used to work in the automotive/heavy machines industry and saw many engine block prints.
I wish I had easy access to the up to date ISO standards as you apparently do. I do have old and new books on the standard though, naturally they will suffer from the same issue we all have here, even with the large volume of our version: "what does it mean", ISO 1101 gives less direction than ASME.
Frank
If we say it is a valid spec, then you have to establish the center line of a cone which is going to be very tricky. Can you section the part to inspect it? If you can you could use an optical comparator to pick up a center points at 2 depths to establish the center line. If you can't section the part you are going to have to use something that can scan the part like a smartscope. $$$.
I can envision a gage/tool that would pick up two gage diameters to establish a centerline for the conical feature...but there is no guidance on the print to establish the datum targets (gage diameters).
On our CMM, our cone measurement command outputs the C/L of cone. That C/L can be evaluated for conditions such as perdendicular.
If our CMM didn't have that command, I would take two diameter measurements; one near bottom of cone, and one near top of cone. The center points of the two diameters would then be used to create a cone C/L, and could then be evaluated.
If I didn't have a CMM, I would use two different diameter ball bearings. The two ball bearings would tell us angle, breakout dia and C/L perpendicular.
At 11.5mm max dia, it's going to be hard to get a good reading with a CMM at more than 1 diameter, and even then it's going to be subject to the surface form. I'm envisioning two microballs on a stick; the small one is fixed at the end and the larger one can slide along the stick until it seats in the conical taper. You then probe off the stick which projects above the part as if it were a projected tolerance zone. I know it's ugly and the repeatability is questionable, but it's an idea.
Adding to or clarifying what JP posted above, ISO now prohibits the appending of datum callouts, fcfs and such to centerlines (as ASME suggested in the first place). Also, ISO 2768 is primarily a size-tolerance standard based on limits & fits essentially. There is some guidance for what it means for orientation, etc., but it's rubbish.
Here is a picture of the shaft, cone, and 2 each balls.
Small ball is 3mm, Large ball is 10mm.
Using surface table, height gage with scribe, and knee block: measure position of both balls in all 3 axis.
The measurement results and trig will show condition for perp, angle, and cone position.
