Aligning groups of holes to another hole pattern? 3

[ShaggyPE]

First off, let me thank you for taking the time to read this. Please see the attached pdf.

My goal is to align the small holes to the larger holes. The small holes create a cross hair type pattern. I need the accuracy of the location ON the cross hair to be held closer than the accuracy ALONG the cross hair.

Image 1:
I have disregarded the looser tolerance along the axis and just forced the part to be held to a tight tolerance unnecessarily. Datum D (applied to the 2X large hole pattern) defines the two midplanes of the hole pattern (horizontal and vertical).

Image 2:
Datum D is assigned to the 5.00 dimension separating the two big holes. This identifies the midplane (vertical) between the holes as the datum. How do I define the horizontal plane between the holes as a datum?

-Dustin
Professional Engineer
Pretty good with SolidWorks

 

[nrostrander]

Dustin,

Perhaps you could could look into defining datums "C" and "D" on your two larger holes and use them to create your positioning datums for the center smaller holes. I attached an example using your part.

May I also recomend looking at the following site for another example of using two holes to define the datum referance frame:
-

http://www.tec-ease.com/gdt-tips-view.php?q=242

-



V/R
Nathan
CAD Technician/ISO Director
Compass Systems, Inc. (

http://www.compass-sys-inc.com/

)

 

[dingy2]

Dustin:

When you qualified the 2 holes for datum D, both holes will become a pattern which controls not only defines the vertical but also the horizontal planes. Your drawing is correct as far as I am concerned.

Certainly, you could have had one hole as datum D and the second hole as datum E. All dimensions would come from datum D while the tertiary datum E is for orientation. Having the pattern of 2 holes as shown in your sketch does exactly that.

Dave D.

http://www.qmsi.ca

 

[Belanger]

Just a couple of fine points on the original two sheets: If you go with the scheme on the first page, I would probably put the "M" modifier after D where it is mentioned in the feature control frames. This is just from the point of practicality, but not written in stone.

For the second page, it's not clear what datum D is. The datum symbol seems to imply that it's the center of the 5.00 dimension, but I suspect you mean it to be the two holes, similar to the first sheet.

You are probably looking for input on the two philosophies in general, so I'm sorry if I'm sidetracking you with little stuff.

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

 

[ShaggyPE]

Thanks everyone.

nrostrander,
Thank you for taking the time to create the sketch. I did some further research last night and came to the same conclusion as you. It is good to get some corroboration.

dingy2,
The hole pattern being datum D (first sketch) was an acceptable methodology. Ultimately I was trying to devise a layout that would allow me to loosen the tolerance in one direction while maintaining the tight tolerance in the other.

Belanger,
Thanks for the input as well. The intent of datum D on the second sheet was to identify the midplane of the 5.00 dimension.

Ultimately I have moved forward with a similar methodology to the one illustrated by nrostrander. I am open to comments on that as well.


-Dustin
Professional Engineer
Pretty good with SolidWorks

 

[Belanger]

Sure, that's fine. However, a datum can't really be derived from the 5.00 dimension, so I would suggest a change there. Depending on the intent, the datum should be tagged with the two holes, but not the distance between them.

However, you may already have those two holes as datums (C or D or whatever), so I don't know if there is any value in even trying to make the 5.00 a datum.

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

 

[pmarc]

I just have to ask for clarification. What is the intent actually?
- to define different positional tolerances of whole pattern in orthogonal directions and in the same time to keep spacing between the holes tighter?, or
- to define different spacing between holes within a pattern for horizontal and vertical holes?

Sorry if this sounds stupid but I can't infer it from the discussion and attached sketches.

 

[ShaggyPE]

Belanger,
The midplane is only being used to apply the "tight" tolerance to the vertical set of holes and the "loose" tolerance to the horizontal set of holes.

pmarc,
The goal is to allow for a looser spacing tolerance between the holes while maintaining a tight tolerance for the linear patterns of holes... relative to the two .250 holes (not part edges/midplanes)

i.e. very much inline but spacing doesn't matter so much.

-Dustin
Professional Engineer
Pretty good with SolidWorks

 

[Belanger]

If the midplane is desired as the theoretical datum, then the datum symbol should be attached to the holes themselves. Can't have it directly with the 5.00.

See ASME Y14.5-2009 paragraph 3.3.2 for how to place the datum triangle symbol. I think you're trying to do as they mention in subparagraph (b), but notice that it says "...an extension of the dimension line of a feature of size..." The 5.00 is not a feature of size. What I'm suggesting is closer to what the standard shows in Fig. 4-39, where datum B can be thought of as the center of the two small holes.

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

 

[pmarc]

Dustin,

Thanks for clarification.
In this case please take a look on attached picture.
I have used the concept of bidirectional positional tolerancing that is shown on fig. 7-28 in Y14.5-2009 or fig. 5-41 in Y14.5M-1994.
I think it is capturing your intent quite well.

http://files.engineering.com/getfil...4-937dd3ca0ccc&file=pattern_bidirectional.JPG

 

[ShaggyPE]

pmarc,
I have used bidirectional tolerancing on slots just like that... I never would have thought of showing it that way for holes... but there it is in Y14.5M. I think this methodology is more clear than the previous one. Thanks.

Belanger,
Thanks again for the info. I only have a copy of Y14.5M-1994. Para 3.3.2 appears to be the same. I am assuming Fig 4-39 (2009) is similar to Fig 4-22 (1994)... where a hole pattern is identified as the datum.

I am not convinced the 5.00 is NOT a feature of size. From 1.3.17 (1994) Feature of Size: ...two opposed elements or opposed parallel surfaces, associated with a size dimension. If the 5.00 isn't a size dimension... what would it be? Is there a formal term? Location? Spacing?

-Dustin
Professional Engineer
Pretty good with SolidWorks

 

[Belanger]

In 1994, I guess 4-22 would work (pattern as a datum), although I was thinking of the one that is 4-27 (two holes forming the datum).

A feature of size can be thought of this way: something that you can grab onto and measure with calipers or a micrometer. Since the 5.00 is the distance between two non-physical points, it can't be grabbed onto. I guess it can be confusing because they don't have an official definition for "elements," but it is meant to be something physical.

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

 

[ShaggyPE]

Off original topic... but still regarding the "feature of size"... would it change anything if it were dimensioned off of the edges of the hole vs. the centers?

-Dustin
Professional Engineer
Pretty good with SolidWorks

 

[Belanger]

Yes, edge-to-edge of the holes would qualify as a "feature of size" (although the way that holes function, that would not be common).

It would change things because the actual radius of each hole would have a direct impact on the distance between them (think of calipers pinching across that rim-to-rim span). Calling the two holes a group datum (a la Fig. 4-27 in 1994) doesn't see the same impact from the holes' actual drilled sizes.

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