Datum shift? 1

[Kennycrft]

Could someone explain to me on how datum shift works?
I was checking out this site:

http://www.tec-ease.com/tips/november-98.htm

and found some info on it, but Im still confused.

for example, the 4X dia. .010 +/-.2 dimension. w/ a positional tolerance of 0.3

How is this different from calculating bonus tolerance?
What changes when you have the modifier in the datum reference? (in this case, the MMC symbol in datum B)

Thanks for your help.

 

[PaulJackson]

Kennycrft,

The attached presentation shows typical abbreviated layout inspection outcomes for measuring and recording position deviations with regard to variable position tolerance limits and variable limits for datum shift. Hope it helps to explain datum shift.

Paul

 

[PaulJackson]

Try again

http://files.engineering.com/getfil...-9ccd-a47c0f333124&file=PatternFitting(M).pdf

 

[Michael854]

Kennycrft,

I think by the "datum shift" you are really referring to datum displacement. Datum shift is a slang term...but Datum displacement has a definition in Y14.5.

I think most novices who try to read the actual Y14.5 wording of datum displacement end up confused...

So...I'll offer a non-Y14.5 definition that I think might make it easier to understand. First...two terms:

1. Datum - theoretically perfect...from which measurements are made.

2. Datum Feature - features on the part...used to establish Datums

Datum displacement is when the Datum feature is not in the same spot as the Datum.

One situation where datum displacement occurs is when physical checking gages use fixed sized pins to hold datum features of size. As the hole gets bigger, the part can wander a bit on the gage.

Michael
GDTP-S0470

 

[Michael854]

Kennycrft,

Oops..It seems I forgot to answer the second part of your question.

Assuming we are talking about MMC...The bonus tolerance is the amount of additional tolerance allowed to the degree the hole is larger than its MMC size.

Remember the Datum for a Datum Feature of Size is a perfect pin at the MMC size. So...at MMC, there is no datum displacement possible...but when the hole departs from MMC, the amount of possible datum displacement is the bonus tolerance.

Modifiers?
Having a modifier in the Datum Reference Frame makes a big difference.

I just walked through when you see the MMC modifer in the DRF...

But with no modifiers...everything is at RFS...no datum displacement.

Hope this helps,

Michael
GDTP-S0470

 

[SeasonLee]

Datum Shift Calculation.
Let’s begin from Datum B
The datum simulator=Virtual condition=MMC hole size – callout tolerance=Ø19.8 - Ø0.2=Ø19.6
Max datum shift=Difference on hole size+callout tolerance=Ø0.4+Ø0.2=Ø0.6

Virtual Size Datum B Datum B Actual Size Allowed Displacement of Datum B
Ø19.6 Ø19.6 Ø0.0
Ø19.6 Ø19.7 Ø0.1
Ø19.6 Ø19.8 Ø0.2
Ø19.6 Ø19.9 Ø0.3
Ø19.6 Ø20.0 Ø0.4
Ø19.6 Ø20.1 Ø0.5
Ø19.6 Ø20.2 Ø0.6

The bonus of the four-hole pattern
Virtual condition=MMC hole size – callout tolerance=Ø9.8-Ø0.3=Ø9.5
Max bonus tolerance=Difference on hole size+callout tolerance=Ø0.4+Ø0.3=Ø0.7

Virtual Size 4 Hole pattern Actual Size 4 Hole Pattern Bonus Tolerance
Ø9.5 Ø9.5 Ø0.0
Ø9.5 Ø9.6 Ø0.1
Ø9.5 Ø9.7 Ø0.2
Ø9.5 Ø9.8 Ø0.3
Ø9.5 Ø9.9 Ø0.4
Ø9.5 Ø10.0 Ø0.5
Ø9.5 Ø10.1 Ø0.6
Ø9.5 Ø10.2 Ø0.7

For example:
Datum B produced at Ø19.9, the 4 hole pattern hole size is Ø10.1 (actually cannot be same size for all holes), most will think this way:
The bonus of the 4 holes is Ø0.6 ( from above chart ) at Ø10.1
The datum shift is Ø0.3 ( from above chart ) at Ø19.9
The total allowable positional tolerance=bonus + datum shift=Ø0.6 +Ø0.3=Ø0.9
You are totally wrong if one calculated this way, there are three ways can be utilized:
1. Appropriate software on CMM
2. Paper gage
3. Functional hard gage

Unfortunately, our company CMM software doesn’t support datum shift calculation, normally I will choose hard gage for incoming inspection while paper gage used on FA evaluation. It’s a simultaneous requirement on the 4-hole pattern and outside diameter on this tip example, the best and easy way is check by functional hard gage.

SeasonLee

 

[dingy2]

I don't like to use the term "datum shift" and some of the wording in both ASME Y14.5-94 and now in ASME Y14.5-2009 is really somewhat confusing.

I will try another way.

Datum B is a hole and what goes in this hole during assembly? Probably a bolt which is cylindrical. If the datum B hole was made at its smallest allowable size, then the bolt just fits into the hole. If the hole was made towards its largest allowable size, then there would be lots of slop when inserting the bolt and now the part can be moved in any direction to check the position of the 4 holes. That would be real life during assembly.

The amount of part movement is the difference between the actual size of the datum B hole and its MMB (maximum material boundary - 2009 standard term) which in this case is 19.6 mm as per SeasonLee information above.

If the datum hole B was not in MMC, one would have to place a tapered pin in this hole locating on the ID circumference. The part has no movement whatsoever. This is in RFS (regardless of feature size) and would be applicable if, during assembly, one placed a tapered pin in the hole. Of course, that doesn't happen so having the datum B hole at MMC reflects assembly condition.

Dave D.

http://www.qmsi.ca