locating hole from a different plane

[greg2835]

Attached is a sketch for trying to locate a hole relative to another hole that is in a different plane with a looser +/- tolerance. Essentially what I am trying to say in the FCF is "this hole is to be parallel to A and located vertically from it's respective basic dimension, it's center is to be in line with the center of the looser hole, and it is to be parallel to datum C with a location tolerance of .005"

I hope that makes sense and sorry if my wording is a little weak (in the process of learning). All comments and questions are most welcomed.

Thanks,

Greg

 

[pmarc]

The position FCF in question is correct and satisfies the intent described.

I would be more worried about direct +/- dimensions used to locate datum hole B. This is a textbook example of dimensioning ambiguity.

 

[mkcski]

greg2835

I agree with pmarc and would like to add the following: +/- dimensioning cannot be used with position control - BASIC dimensions are required to define the true position location. See last paragraph of 7.2 below.

Additionally, Datum B is a feature-of-size and design consideration should be given to material condition modifiers - MMB or LMB datum simulation. As shown RMB (variable simulation) applies per Rule #2


7.2 POSITIONAL TOLERANCING
Position is the location of one or more features of size
relative to one another or to one or more datums. A positional
tolerance defines either of the following:
(a) a zone within which the center, axis, or center
plane of a feature of size is permitted to vary from a true
(theoretically exact) position
(b) (where specified on an MMC or LMC basis) a
boundary, defined as the virtual condition, located at the
true (theoretically exact) position, that may not be violated
by the surface or surfaces of the considered feature
of size.
Basic dimensions establish the true position from
specified datums and between interrelated features. A
positional tolerance is indicated by the position symbol,
a tolerance value, applicable material condition modifiers,
and appropriate datum references placed in a feature
control frame.

Certified Sr. GD&T Professional

 

[pmarc]

mkcski,

If the datum feature of size B is indeed trully functional secondary datum feature for this part (let us assume that no other datum features than A, B and C are needed), then it is not position tolerance that needs to be looked at in first place. Datum feature B most likely needs perpendicularity tolerance relative to A. After having A and B established and properly controlled, the other features of the part (including datum feature C) should receive appropriate geometric tolerances. For that it is even possible that those two .25 dimensions (regardless if basic or directly toleranced) will not be needed at all.

 

[mkcski]

parc:

Thanks and I agree. Not knowing the knowledge level of the OP, I was just trying to clarify the application of BASIC dimensions.

Yes, the relationship between the datums is not qualified.

The hole is be "on" the center plane from datum B so the left-right BASIC dimension would be "0" and not shown.

Certified Sr. GD&T Professional

 

[greg2835]

Thanks guys, this is good for me as you are using terminology that I am just starting to get a grasp of.

Let's say the hole for datum B is for a pin (though my size tolerance would say otherwise) but let's say it's for a pin and thus I would like to keep the position tolerance relative to B RFB. I will also add a perpendicular tolerance to datum feature B since it is rather ambiguous without it (might ask a question about this later). Is it still inappropriate to have the +/- .25 dims to locate datum feature B? I guess I could see why it would be since one could ask, "what are those dims *actually* being measured from?"

Thank you in advance,

Greg

 

[greg2835]

and I meant RMB, not RFB.

 

[mkcski]

greg2835:

I would recommend using position the control the location of the Datum B hole itself. I would suggest using Datum A as the primary datum (3 motions controlled) , the width as the secondary Datum and not one side of the width like Datum C (two motions controlled), and one end as the tertiary datum (one motion controlled). If the design requires it, you could make the position tolerance "large" and refine the implied perpendicularity by adding a separate perpendicularity control at a "smaller" value. Note: composite position is not allowed as it can only be applied to two or more features

Certified Sr. GD&T Professional

 

[Belanger]

Rather than positioning that datum feature B, it's also possible that the outside walls of the part are profiled back to B.

In other words, maybe datum B is the center of the universe for the part, and everything else is located to it. Just tryin' to rock the boat

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

 

[mkcski]

John-Paul's alternative should certainly be reviewed against design requirements. Locating the edges from features "in" the part is "backwards" from the traditional approach of features located from the edges - mainly because mfg machines the edges first and locates the features from the edges. But the dimensioning schema does not have follow mfg methods. The part has to meet drawing requirements no matter how it is mfg'd.

Certified Sr. GD&T Professional

 

[pmarc]

Dimensioning the part based on how it is, or most likely be, manufactured is "backwards" from the approach presented in modern dimensioning and tolerancing standards, like ASME or ISO.

 

[drawoh]

I would be more worried about direct +/- dimensions used to locate datum hole B. This is a textbook example of dimensioning ambiguity.

Strictly speaking, the [±] tolerances are locating the outside edge from the hole, not the other way around. This is an excellent place to use profile tolerances.

--
JHG

 

[pmarc]

Strictly speaking, the ± tolerances are locating the outside edge from the hole, not the other way around. This is an excellent place to use profile tolerances.

I am curious, how can you be so sure about that? Is it because B has been referenced secondary and C tertiary in the position FCF for the other hole?

This is an excellent place to use profile tolerances.

Perhaps, but again, why are you so sure about that without knowing how the part really functions? Theoretically, couldn't the (.500) width be controlled with position tolerance wrt A|B and then one of its side faces be assigned datum feature C? Or, as already stated by mkcski, the entire width, not only one of the faces, is a better candidate for datum feature? Who knows? Too many if's, in my opinion.

 

[drawoh]

pmarc,

Obviously, I don't know the original design intent. I am assuming that any dimension that originates from a datum, defines the other feature. Yes, the base could be an FOS positioned on the datum hole.

--
JHG

 

[greg2835]

It brings me great joy to see many different people contributing. It is greatly appreciated, and thank you mkcski for your clarity for my infant GD$T mind

Allow me to provide some context for what the part is for. Let's say this part will sit on a flat table on datum feature A. There is a pin in the table that datum feature B mates with. The hole parallel to A in the part is used to hold an arm that is holing an optic. A laser is generating a beam that is targeted to pass right over the pin in the table. The idea is to create tolerances to ensure that the beam hits the optic in a small allowable area. Hopefully that made sense. The values I am using for size and tolerances are completely made up and are there to give a sense of what is looser and what is tighter.

Attached is a rev2 of the dwg in accordance to what mkcski suggested in his previous post. I also added a parallel tolerance to one of the holes to better control the holes orientation. All comments, questions, and concerns are most welcomed. After this I will also give a shot to using profile tolerance as suggested by others (which will be very new for me).

Best,

Greg

 

[mkcski]

Greg2835:

Looks good to me. I could suggest qualifying the Datums to each other by: adding flatness to Datum A; making Datum D perpendicular to Datum A; and Datum C perpendicular to A and D. You might also apply controls for the two vertical faces if they need it.

Certified Sr. GD&T Professional