Dimension origin and datum 1

[SeasonLee]

Very simple question :

1. Can we add dimension origin symbol on a datum as shown on the attached ?
2. If yes, what are the differences between option 1 and 2 ?

Thanks for all inputs

SeasonLee

 

[Belanger]

I would think it's OK to use the dim origin symbol if it is a concern to have the part measured in that way. It's independent from the datum feature symbol. In other words, the datum feature symbol doesn't add any value to either picture, because it's not referenced in a feature control frame, which is its only job (unless a note invokes datum A for non-GDT dimensions).

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

 

[drawoh]

SeasonLee,

On ASME Y14.5M-1994 and ASME Y14.5-2009, look at Figure_2.5. The origin system can be significant.

If your case, it depends on how you control geometry. If you use profile tolerances, then you will do them from your specified datum_A, and your dimension origin will be irrelevant.

JHG

 

[PaulJackson]

SeasonLee,

If there were actually tolerances for size in your example and the standard applied was ASME then there wouldn't be a difference because the "envelope principle" establishes the maximum material size.

In ISO those maximum material sizes could inflate to size plus the limits imposed from the flatness... unless of course the "envelope principle" specified with (E).

The ISO standards commonly state that larger, longer, wider, surfaces are physically selected rather than the opposite for measurement orientation when datum features are not specifically identified... so even in ISO without the "envelope principle" specified there are safeguards to prevent the measurement amplification effects highlighted by ASME Y14.5M-1994 figure 2.5.

If your figure illustrated a tolerance that was not applied to opposed elements of feature size then figure 2.5 aptly describes the possible outcomes of measurement orientation differences that can be limited by the origin symbol.

Paul

 

[SeasonLee]

Thanks for all of your inputs, Balanger, drawow and Pual.

The print revised for discussion purpose, let me interpret this way:

Option 1---The bottom surface is primary datum surface, therefore I will measure the dimensions from this surface. There is a tolerance of ±0.2 for all linear dimensions, I will assume this ±0.2 tolerance shared by both bottom and top surface, and the flatness 0.1 will be exactly same as the tolerance shared by the bottom surface.

Option 2---There is a dim origin symbol on the bottom, the dim will be measured from this surface to the top, and the linear tolerance ±0.2 will be on the top surface, that means the entire tolerance zone ±0.2 is on the top surface. The flatness control is a geometric tolerance control on the bottom surface, there is nothing to do with the overall height dim measurement.

Option 3---This case will be same as Option 2 since the datum feature is independent from the dim origin symbol.

Question: For Option 2, there is a datum feature symbol on the bottom, I thought all of you will measure the dimension from this datum surface even without the dim origin symbol on the bottom, no one will measure it from the top surface for sure, is it superfluous for the datum symbol here in case the dim origin symbol had been included on the bottom surface.

Thanks again

SeasonLee

 

[pmarc]

SeasonLee,

Let me add some comments to what you wrote:

Option 1 - assuming that datum A is not referenced anywhere else on a drawing of this part, the symbol of it is not neccessary at all.
Correct approach is that only dimensions related to a datum reference frame through geometric tolerances should be measured in a DRF. If a dimension is not associated to a DRF with a geometric tolerance, there is no specification on how to locate a part in a DRF.
So in your case dims. 15 and 35 should not be measured in relation to datum A. Simple caliper measurement can be taken (of course if opposed elements exist). However if you leave A on the drawing, I am pretty sure that most of inspectors will put the part on flat surface simulating A and then measure the height of the 15 and 35 features. Doing that they will simply associate a part with DRF.

Options 2 and 3 - you are right that by assigning bottom surface as an origin of measurements for both dimensions, +/-0.2 tolerance zone will be on the top of both features (it is clearly shown on fig. 2-5 of Y14.5M-1994). But again, if datum A is not referenced anywhere else on a drawing of this part, you simply do not need it. Placing origin symbol on the drawing should be sufficient information for inspector which surface the measurements should be taken from.

So in my opinion Option 3 is the most correct one.

 

[dingy2]

SeasonLee:

If there is not a reference to datum A in a FCF on the drawing, then option #3 is correct.

Dave D.

http://www.qmsi.ca

 

[SeasonLee]

Thanks for all comments, the print revised again to add DRF with geometric tolerance.

Is it necessary to indicate which surface functions as the datum feature for the inspection ( of height 15 and 35 ) in case the DRF already specified on the print as shown on option 2 ?

SeasonLee

 

[Belanger]

Probably Option 2...

Sorry to nitpick -- be sure to add the M symbol after the zero perpendicularity. Then perhaps the M after "B" where it is referenced in the position tolerance -- but that one depends on function.



John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

 

[pmarc]

SeasonLee,

Option 1 - despite datum A is clearly specified on the drawing, dims. 15 and 35 still should not be measured in any relation to datum A.

Option 2 - if you want to have bottom surface as an origin of 15 and 35 measurements, it would be much more according 'state of the art', when you make these dims. basic and apply profile of surface |ProfileOfSurf|0.2|A| to both top surfaces. Then it would be clear that location (height) of these two surfaces is relative to A.

Hope this helps.

 

[pmarc]

SeasonLee,

A few words of addition and correction of previous post:
Since general tolerance on linear dimensions is +/-0.2, the value of profile tolerance could be 0.4 instead of 0.2, of course if you decide to use profile. However if not, I think your option 2 is also legal and acceptable.

As John-Paul said, M modifier in tolerance portion of perpendicularity control of datum feature B is a must. Using M after B in position tolerance depends on function of the part.

 

[dingy2]

Figure 3-30 page 47 of ASME Y14.5-2009 shows exactly the same condition as you have in option #1.

Dave D.

http://www.qmsi.ca