My interpretations is that you are trying to use two different dimensioning schemes to document the part.
Ordinate Dimensioning utilizes a "0" point and then location dimensions based on the distance from said point
Basic Dimensioning are most commonly accompanied by a positional tolerance on the feature being dimensioned.
Having said this, using your combined dimension scheme there isn't any right/wrong way.
I would choose one or the other.
Just my 2¢
I see arrow heads. In Ordinate dimensioning there are no arrowheads. What are those there for? Your datum A is in the wrong place. Datum A is the hole. The hole would be the datum and would be the first hole placed and or indicated to by the machine or by QC in checking your part. "0" would not need to be a basic. Left to right dims would be the same where the "0" is the center of the hole. In placing the datum "A" on the edge of the hole it is saying the hole is the feature and datum.
My original example image was far too simplified and may have caused misinterpretations. Here is a much more detailed example of the situation I'm asking about:
In this example you see that the large bore itself is Datum A, and the horizontal plane centrally intersecting Datum A is Datum B (this datum strategy is inherited, not of my making). The three smaller holes are controlled by the tolerance zone indicated in the position callout, and as such they are dimensioned with X and Y TEDs (basic dims). The question actually revolves around the hole directly to the left of the large bore...
My colleague contends that the position callout does not apply vertically to the hole to the left of the large bore because it is not dimensioned vertically by a TED. Thus, he says, it is located horizontally but not vertically, and to correct the situation I need to make the '0' dimension basic, ie, to put a rectangle around it.
My contention is that:
A) the '0' dimension of an ordinate system defines the point from which other dimensions are measured, and cannot itself have a tolerance (though it could extend from a feature that was positioned according to a given tolerance, which the ordinate system would then inherit), and
B) in this particular case, the '0' dimension and the hole itself are clearly vertically located on a stated datum, and by definition a datum is not subject to a tolerance. This datum location applies to the vertical position of the hole by defining its exact vertical location relative to the relevant datum, and therefore acts as a TED. The position callout therefore creates a tolerance zone around the exact location (5.086 horizontally, 0 vertically), obviating the need for any actual declaration of the '0' dimension as a basic or TED, which according to contention A is not allowed anyway.
So ultimately the question is: Do we need or can we 'legally' place a rectangle around the '0' dimension of the vertical ordinate system? Does it even make a difference?
Your contention is correct. There shall not be a box around a "0" in a dimensioning scheme. It is not subject to a tolerance, it is the theoretical location from which all other dimensions are relative to. If "0" were allowed a tolerance then that would be added to the tolerance of the dimension referenced from it. That makes as much sense as an elephant in a china shop. So, just because someone else screwed up and made the center of the part a Datum, does that mean you have to follow? A datum is a feature, what feature is datum "B" associated with? I don't see it associated with anything. In the machining world (which the designer or engineer better damn well know) datum "A" is the bottom of the vise (and so the bottom of your part). Datum "B" is the top edge of your part (or some prefer the bottom edge) which is the non-movable part of the vise. Datum "C" is the left edge of your part (or the vise stop). That is where "0-0" is on the CNC machine. Anything other than those are then "D" and forward. In your case if you don't care about all the other datums then you can go ahead and make your hole datum "A". Datum "B" is irrelevant, means nothing, remove it. What you are looking for is that holes are relative to your datum "A". If you want datum "A", (your hole) to be perpendicular with some sort of accuracy then you need to establish the machining world standards as mentioned above. If you don't care about the edges as far as location then establish datum "A" as mentioned above and put basic dims on everything associated with your hole datum which now becomes datum "B". Your datum hole (which ever you chose to do) has a locational tolerance to the edges of your part. You may not care about those since it appears your only concern is the relativity of the holes to your large datum hole. Again, datum "B" means nothing and it should be removed.
Now as for the .001 positional tolerance you have shown, how much money you got? Cause no one will ever be able to hit that. That's a .001 dia circle you are asking to hit with the center of the hole. Are these hole "S" (regardless of feature size)? Positional of .007 is a .005 dia tol circle.
By stating the hole as Datum A, two orthogonal planes are created, intersecting at the theoretically exact/perfect axis of that hole.
The basic dims are from these two planes, so the ordinate zeroes are irrelevant.
Therefore do not basic box the zeroes.
But...one of the (3) .653 holes is dimensioned to a zero value, therefore this zero is a basic dim for that .653 hole's position.
So, box this zero.
Also, the dimension origin arrows in your OP aren't needed and shouldn't be used,
Lastly, as stated previously, the .001 positional tolerance seems fairly tight, not knowing your design intent.
Each .563 hole's axis (of any shape/angle) must reside in a .001 diameter cylinder which has a height equal to the thickness of your part,
The thickness isn't stated, but the thicker it is, the tighter the perpendicularity (and shape) of the axis becomes to maintain positional spec.
As a suggestion, consider adding an MMC to the positional frame so any departure from the .563 size can be used to open the position tolerance.
The hole size tolerance isn't specified here, but it usually can be added in as MMC without a loss in mating.
I hope this helps.
Kevin, I don't agree with all that you say, but he has options depending on what he is trying to accomplish. I don't agree that "O" gets a box, makes no sense, now you are trying to apply a tolerance to that using a feature control (geo tol). I don't see that happening. Also MMC is implied in the ANSI STD's, it is not required to state so in the feature control box. I agree with you as I stated above on the .001 positional control. No one can ever make that part and I doubt anyone can even measure it to know if it is correct. Even in critical optics world it won't ever happen. That's a weird hole size 1.861. Not American or Metric or dowel pin ream size. So, right off the bat, that's a bored hole. And to be accurate, the .653 holes which are also not American or Metric will have to be bored holes. So, some accuracy is being instilled into the part, but it ain't gonna be .001! :-)
Some related items:
1) You've indicated your larger hole as the primary datum and it's partially duplicated by datum B (I didn't view the whole image for Diatribe I).
By making your hole primary, this part must be fixtured (for fab & inspection) on this bore, preferably a 3-point contact or by an expanding collet.
Datum B adds nothing so this part is located on the hole only.
There's an implied 90° to the edges, so
As a suggestion, make the base of this part Datum A, the top edge B, the left edge C and the large hole D.
Relate B & C to A and then relate C to A, B & C (in that order). Position the .653 holes to D & A (in that order).
This provides the best bearing for fixturing.
2) As a general rule, I run dependent tolerances at 3:1.
What I mean is, if a toleranced surface depends upon another surface to maintain its bearing, the dependent tolerance value is at least three times the tolerance of it bearing surface's tolerance.
This isn't a hard & fast number/rule, but you will need some tolerance adjustment for surfaces that have others depending on them.
It's tough to hold a tight tolerance when fixtured against wobbly surfaces.
See diatribe #3 for an example.
3) Your flat datums need flatness tolerances and the large hole datum needs a cylindricity tolerance to be proper bearing surfaces.
Per diatribe #2 and your .001 positional tolerance, the flatness and cylindricity tolerance is .0003, small indeed.
As a suggestion, start tolerancing on your datums surfaces (these will require the tightest of the design, cost, etc...) and then tolerance the surfaces that depend on these. And so on.
4) Another practice I do is to compare a feature's form tolerance to its size tolerance.
Again, nothing firm/official. Just a tool to help me review tolerances.
The .563 holes aren't toleranced for size, so assuming a default 3 place decimal is +/-.005, the hole size tolerance is running 10:1 to the positional.
Seems high, but it could be needed, dunno. That's point of evaluating this ratio, are you being overly strict on size or form?
I hope this helps.
Bruce & Brian,
For the most part, I agree with Bruce's interpretations. The application of GD&T is often interpreted differently depending on the individuals involved. Because of this, you should always refer to the specification; "ASME Y14.5", Dimensioning and Tolerancing to settle disputes.
A couple of things I'd like to mention here with regard to GD&T and your case:
- Basic dimensions are basic. (not ordinate) They are considered exact.
- Most cases of GD&T involve datums, usually primary, secondary and tertiary. They are also considered exact.
- The application of tolerance defined by the feature size and its positional tolerance.
- There are absolutely no reference to the identification of "zero" with respect to GD&T.
- Zero cannot be basic because it does not exist. GD&T establishes/identifies what datums, conditions, and features are used to dimensioned a part.
Lastly, to better answer your questions it would be helpful to see where the part is used and how it fits/relates to other parts in an assembly.
Many thanks to all who have contributed to this discussion. It's great to be able to pick the brains of so many experienced professionals in the field!
Allow me to clear up a few points that seem to be catching people up:
- The arrowheads which appear in my first example image were put there automatically by SolidWorks. It was apparently using a different drawing template than the one we officially use (and which is of unknown origin), and that template seems to be set to use arrowheads when creating ordinate dimensions. Those arrowheads were not put there by my design, but I ignored them because their presence does not in any way bear on the primary question.
- The values of the dimensions and tolerances used in either of my example images are entirely arbitrary. I made no attempt to use values that were reasonable or logical in a real-world sense and as such any discussion of whether the hole sizes are common or whether the tolerances are manufactureable are entirely moot. Again, I ignored the values that randomly appeared when I quickly ginned up the example because the exact numbers do not bear in any way on the question I was asking.
- The datum scheme shown in the second example image is taken from the actual part in question (which I can't post due to IP protection issues), but it is incomplete. The actual part uses a major internal bore as Datum A because that bore is the journal for the main shaft of a gear train assembly, and the locations of all other components must be controlled relative to that feature to ensure proper fit and functionality. Other datums (data?) occur in the original part, but I left them out because, again, they do not bear on the primary question.
- Some have questioned the purpose of Datum B, which seems to be redundant to the existing Datum A. I believe the purpose of Datum B is to provide a rotational reference which is not provided by Datum A, since Datum A is a cylindrical feature and provides only X and Y location reference without bearing on rotation. I may be wrong in this interpretation, but as I said, I inherited the scheme, so I can't speak directly to its intended purpose (and it doesn't bear on the question!).
For the record, the primary question is whether or not the '0' or base callout of an ordinate dimension system is allowed to be defined as basic, and if so, whether doing so is necessary in the example I gave in order for a feature placed on that '0' line (and consequently on the datum) to be effectively controlled by the tolerance zone specified by the position callout. In other words:
Should I put a box around the '0' on the vertical ordinate system?
As a final note, I will mention that the actual part is a casting, with no reliable external edge that would serve for fixturing or measuring, and thus the datums (data?) are created to reference the internal machined features instead.
Thanks again for all the input!
Thanks for the clarification.
Like I stated originally, you cannot mix ordinate with basic dimensioning schemes. No zero exists in this fashion using GD&T.
Having said this, I have seen companies dimension parts how ever they want and yours is no exception.