when to use hole pattern as datum feature 3

[bxbzq]

I see many times, from function or assembly standpoint, hole pattern (bolt holes, pin holes) constrains degree of freedom of a part, but they are not datum feature. So I'm wondering if there is kind of rule of thumb or tip as to when to use hole pattern as datum feature. Another question, is hole pattern manufacturing or inspection friendly as datum feature?

 

[powerhound]

To your first question: I don't know if there's a rule of thumb.

Second question: If using a hole pattern as a datum feature, the easiest way is to reference it at MMC. That's the only way it is shown, or even talked about, in the standard. This doesn't mean referencing a hole pattern at RFS is wrong but it's definitely a tough check. That's been hashed over in this forum before.

Powerhound, GDTP S-0731
Engineering Technician
Inventor 2010
Mastercam X6
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[Belanger]

If all holes are of equal importance, then they should be identified as a (pattern) datum feature.

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

http://www.gdtseminars.com

 

[MechNorth]

It comes down to functionality; if all holes act simultaneously or with equal chance of "contact", then they should be used as a pattern, otherwise (for example, one hole slightly tighter than the others) select a single feature instead.
Y14.5M-1994 only permits a pattern of features to establish a datum when they are referenced at MMC. Not sure why, but suspect a bias toward hard-gauging. That requirement was lifted in 2009.
I don't know about friendly or unfriendly for manufacturing or inspection; there are so many different fabrication techniques (simultaneous vs individual feature fabrication) and metrology techniques available that it is a case-by-case question.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[PaulJackson]

So I'm wondering if there is kind of rule of thumb or tip as to when to use hole pattern as datum feature

Use it when they "as a pattern" functionally constrain one or more of the part's orientation and/or translation degrees-of-freedom. If you choose a surrogate you will have to stack through the surrogate unnecessarily to predict chosen clearance/interferences.

is hole pattern manufacturing or inspection friendly as datum feature?

[ol A]
[li]Manufacturing can/may use any feature(s) they desire to fabricate the piece, in fact the pattern can be the final operation in the process... they just have to insure that when the piece is interrogated from the DRF that those features establish the related must conform to it.[/li]

[li]If the datum pattern is referenced "MMC" and the feature tolerances "MMC" and you intend to use attribute gauging then the application is fairly straight forward... The gage sucessfully fitted over the datum features and the toleranced features simultaneously would signal a "go" conformance you would just need then to check each local size of the datum features and related features to verify that they do not exceed their LMC size.[/li]
[li]If the datum pattern is referenced "RMB" and the feature tolerances "MMC" and you intend to use attribute gauging then the gauge details contacting the datum pattern features get more complicated in that they must expand/contract at their basic pattern locations until sequential uniform expansion constraining the eligible degree-of-freedom is achieved. The gage then if successfully fitted over the related features signals a "go" conformance you would just need then to check each local size of the related features to verify that they do not exceed their LMC size.[/li]
[li]If the datum pattern is referenced either “MMC” or "RMB" and the feature tolerances are "MMC" and you intend to use continuous data gauging then Coordinate Measuring Devices often have subroutines where an array of the pattern’s basic coordinates can be compared to an array of the pattern’s measured coordinates and solved for eligible “best-fit” rotations and translations to establish the DRF… then depending how sophisticated the software is written to interrogate the datum feature pattern surfaces for their UAMEs or their RAMEs some software can simulate attribute gauging with DRF mobility for all simultaneous requirements. Many older packages however cannot properly estimate or apply the DRF mobility entitlement unidirectional to all simultaneous requirements so it is best to disregard the option and instead consider the datum reference RMB. Most CMMs have a pattern fitting subroutine that can employed constrain eligible DOF and establish a candidate DRF “bestfit” from the array comparisons.[/li]
[li]In an open layout inspection the skill and experience of the inspector is key. One with experience and knowledge of the process can make rational assumptions, verify them, and set up his pattern balance and interrogation reasonably quick. Barring that most will set on one hole of the pattern and rotate another sufficiently removed from the first according to its polar coordinates and begin the estimation of conformance.

All in all each of these methods begin by modeling the functional relationship rather than a surrogate.[/li]
Paul[/ol]

 

[drawoh]

bxbzq,

I prefer to use the part base and outline as datums. I strongly prefer to use accurate features as datums.

Often, I want to apply sloppy tolerances to my part outlines, and I have an accurate hole pattern. The part outline stays sloppy.

--
JHG

 

[bxbzq]

Thanks to all replies.
I would appreciate it if anyone can show me an example of using hole pattern as datum feature.

 

[Belanger]

Bxbzq -- see attached graphic. The four holes are each positioned to A, B, C, and then they collectively form datum D, which the center hole is positioned to.

Notice that the basic dimensions of 20 and 45.6 could have been tagged to any of the four holes, since they all help form the datum.

The trick is that -- because datum D is made up of a pattern -- it's helpful (I was going to say required, but that's too absolute) to reference datum D with the "M" modifier. That way, if any of the four holes are a little off center (and they will be) then there is slop or "shift" to allow for that.

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

http://www.gdtseminars.com

 

[bxbzq]

Thanks John, is your example from real world application? It probably does not matter, I'm just curious.

 

[Belanger]

It's from some training materials, so it is generic. But the concept is quite applicable to real-world stuff.

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

http://www.gdtseminars.com

 

[SeasonLee]

bxbzg

I like these two pages from Alex's "Advanced concept of GD&T", hope this is what you are looking for.

SeasonLee

 

[bxbzq]

Good reference.
Attached is graph shows my case. There are two relatively tiny pin holes (ø25 vs. ø2964) on the flange surface. The other one is on opposite side of vertical centerplane. In this case, I doubt the pin hole pattern is qualified to be a datum.

 

[KENAT]

The biggest problem I see routinely using hole patterns as datums is that many folks don't really understand what it means. It's a shame to avoid using it for this reason but there you have it.

Unless there's a really strong reason to use the hole pattern I'll often do as drawoh - always with a nagging doubt in my mind that I'm giving in though.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[pmarc]

Kenat,
Sorry for being a little bit sarcastic, but your reply reminds of a statement I often hear:
"I will not apply GD&T on a print, because manufacturer and/or inspector does not understand this stuff at all."

 

[KENAT]

That's basically the reason though pmarc, as much as it bugs me to admit it.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​