Position Control Refinement Dimensions & Datum Establishment

[Jieve]

Hello,

Two questions:

1) Although I have probably beaten this example to death in my posts with GD&T questions, let’s assume I have a flat rectangular plate with four holes in a rectangular pattern. Datum A is the bottom flat face of the plate, datum B the longer side (horizontal) and datum C the shorter side (vertical). I specify 4x Diameter, with a position control frame below: |pos|Diam 0.2|A|B|C|. My tolerance zone for each hole axis individually is therefore a diameter of 0.2 relative to datums B & C and perpendicular to A.

Now I am interested in keeping the each hole tolerance zone within a diameter 0.05mm of each other, perpendicular to datums B & C, but want to allow them to move around as a pattern within the original diameter tolerance of 0.2mm from the datums. I use the following control:
|Pos|Diam 0.2|A|B|C|
|Pos|Diam 0.05|A|

As I understand it, this would refine the tolerance zone between features, as well as the hole axis perpendicularities, but allows rotation of the pattern as well. This is also still a bit confusing to me, because if the tolerance pattern can rotate, are the horizontal and vertical basic dimensions between the holes still horizontal and vertical dimensions when relating pattern features to themselves? What I mean is, what criterion would be used to determine if one hole is within spec relative to another? If the same horizontal and vertical basic dimensions were used as drawn (in other words remained horizontal and vertical) for this determination, since a zero basic dimension is implied between two holes located on the same horizontal axis, the pattern would essentially not be able to rotate and be automatically clocked to datums B & C. However, if the basic dimensions are used between holes but the tolerance zones are rotated, the dimensions are now at an angle and are no longer vertical and horizontal, as specified on the drawing. Can someone clarify this for me?

2) As I have as good as no shop experience I am wondering about datum establishment for things like holes, midplanes, etc. After a previous posting about using slots as datums, something occurred to me. I can envision two ways of determining the midplane datum location of a rectangular part. One shop measures the length with a digital caliper in a couple places, takes an average and divides this by 2. Another has a precision vice type device where the part is clamped so that the respective degrees or freedom are restrained and the midplane datum is derived from the “flat planes” of the vice. As far as I understand, method 2 is the correct one.

Another example. I specify a hole in a thin, flat plate as a datum. One shop measures from an edge to the inside and outside edges of the hole, calculates a centerpoint, as uses this as the datum for reference to other features. Another shop uses a proper gauge pin and measures from the pin to the necessary features as specified on the drawing. I assume number 2 is again the correct method.

For a slot, then, wouldn’t it be necessary to actually use some type of precision pin or plug or something to establish the datum? Wouldn’t something like this have to be fabricated, requiring extra time and money? I’m trying to get an understanding of actual measurement techniques so I can more effectively specify my datum features to achieve the desired function but minimize the work done by the inspectors, machinists, etc. Plus when these guys ask questions, as they often do, I need to be able to adequately explain my reasoning.

Thanks!

 

[Belanger]

For your first question, the basic dimensions that tie the holes to each other are no longer related to datums B and C, so those basic dimensions rotate with the pattern. Think of an electric plug and an outlet: Even if the the outlet is accidentally rotated 20º on the wall, the basic dimensions that tie the holes to each other must be maintained.
For the second question, there are many ways to derive a center, but in general one that uses more of the edge/perimieter is better. What I mean is that calipers aren't the greatest way to find the center because they use only 2 points. For a shaft sometimes a 3- or 5-jaw chuck is used, but the ideal device would be a collet or something like an iris that encircles the feature everywhere. As you say in your last paragraph, it comes down to what's available in terms of equipment, time, and of course money.

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

http://www.gdtseminars.com

 

[Jieve]

So am I correct then, that there is no difference between the ISO control:

|Pos|Diam 0.2|A|B|C|
|Pos|Diam 0.05|A|

and the ASME composite control:

|Pos|Diam 0.2|A|B|C|
| |Diam 0.05|A|

Regarding the second question, are you referring to establishing a hole as a datum feature or just measuring the center location of a hole? I was under the impression that precise equipment is actually necessary when using a hole as a datum feature, although I was also under the impression that this isn't always how it works in reality, as the shop may not have the proper tools, etc. I'm curious how this is done, since I unfortunately don't have much experience in the actual measurement process.

 

[Belanger]

If I recall, ISO doesn't use the composite symbology, so yes those two would be the same. (Even in ASME they would mean the same since there is only one relationship to datum A, but it would typically be shown as one position symbol.)

I was just giving a general comment about how to find the center of a hole. If the hole is meant to establish a datum, however, then we also need to know if there is a "M" modifier involved (at least in ASME) since that would signify that a fixed-size gauge pin may be used even if it doesn't fully contact the hole. Absent the "M" then the precise equipment (i.e., variable gauge) is needed.

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

http://www.gdtseminars.com

 

[pmarc]

J-P,
I agree that even in ASME they would mean the same, but only if single pattern of features is considered.

However, if two or more patterns having identical positional callouts come into play, two single segment FCFs will not be equal to composite FCFs due to the fact that for lower segments of composite FCFs simultaneous requirement by default does not apply, while for bottom frames of multiple single segment FCFs it does.

 

[fsincox]

Jieve,
It does all depend on what datum "A" is, if it is "the classic" perpendicular flat face it is the same, otherwise not so much.
Frank

 

[MechNorth]

Also, J-P and PMarc, if the DRF of the second line of a multiple single-segment has more than just the primary datum, the it also locks down the position wrt the last datum referenced more tightly. Thought this might be important to step beyond the OP so that it doesn't leave a false impression that they are truly the same callouts.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com