Unequal bilateral positioning 1

[JLang17]

I have a hole that is called out with vertical positioning +-.005 and horizontal positioning +.006,-.001. Is there a way to use a positional tolerance (or any GD&T method) to allow more movement in one horizontal direction than the other? Or does the hole need to be centered in the tolerance zone?

Simply put, the hole can move left .001 and right .006. How do I show that with GD&T?

 

[JLang17]

Maybe bilateral wasn't the right word in the subject, bidirectional maybe.

 

[ringster]

JLang,

What version of the Standard is being applied to your documentation? What is the purpose of the hole and what is the interface? It might be a case where positional tolerancing is of little or no benefit.

 

[JLang17]

You know, a better question would be, does Y14.5-1994 allow me to leave it as a plus/minus dimension without applying an FCF?

I'd look myself, but I don't have a copy because my company decided to wait a little bit and get the 2009 version.

 

[ewh]

There is no requirement in the standard that mandates the use of GD&T.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[KENAT]

2.1.1.1 Positional Tolerancing Method. Preferably, tolerances on dimensions that locate features of size are specified by the positional tolerancing method described in Section 5. In certain cases, such as locating irregular-shaped features, the profile tolerancing method described in Section 6 may be used.

Some might interpret the above as a mandating use of either position or profile but many would argue otherwise.

Was the +.006 -.001 calculated from first priniciples/function or are you just trying to translate an existing +- tol of unknown validity into GD&T?

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

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

 

[KENAT]

In terms of your actual initial question, I wonder if you could use position on the whole without the dia symbol. Essentially apply FCF like you would for a slot, one in 'X' and a separate one in 'Y'. I believe you'd have to nominally center the hole in both axis rather it being off set, however from a pass fail criteria this makes no difference.

From a design intent point of view some might argue the unequal +- better captures intent, implying the hole is preferably in the left of the tol zone. However, inspection wise, and hence presumably function wise the scheme would be equivalent except with position you could take advantage of the MMC principle to gain some tolerance.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

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

 

[ewh]

To me, this is like the "TYP" issue; there is a preferred method, but the preferred method is not mandated as a requirement. The give-away is the use of "Preferably" in that quote.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[ringster]

In response more directly to the initial question. The hole does not have to be 'centered in the tolerance zone'.

It may fall anywhere within the zone after it has been properly defined, I do believe.

 

[ewh]

Sorry to keep vering off topic, but I so rarely disagree with KENAT, that I feel I have to explain myself further...
Positional tolerancing IS NOT a requirement of ASME Y14.5-1994. There are requirements pertaining to the use of positional tolerances, but direct tolerancing is allowed.

2.1.1(a) as direct limits or as tolerance values applied directly to a dimension.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[KENAT]

ewh, while I do still use +- sometimes, I believe the section could be interpreted as the 'preferably' meaning to preferably use positional instead of profile but that one of those 2 should be used.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

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

 

[drawoh]

ringster,

The hole does not have to be centred within the tolerance zone, but a GD&T positional tolerance zone is centred about the nominal hole position.

ASME Y14.5M-1994 explains what ± tolerances mean. The OP's description, however weird it is, can be interpreted by a fabricator and an inspector. This is the fundamental purpose of the standard.

ASME Y14.5M-1994 is entitled Dimensioning and Tolerancing. The term GD&T does not appear on the cover, anywhere.

JHG

 

[KENAT]

Should have added 'for features of size'. I certainly am not one of those who thinks almost all tolerancing should be done by surfact profile.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

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

 

[ringster]

JLang,

If this drawing has been prepared IAW 1994 version you cannot simply make all interpretations of the 200X versions apply.

 

[JLang17]

The idea is to translate the existing +- to GD&T. However in this case, it really isn't necessary so if it's not required by the standard I will leave it as is.

The X,Y positional tolerancing as KENAT described would be fine, but that would require changing the dimension value so it lands in the center of the tolerance zone. Very simple, but in SolidWorks, editing a dimension prevents it from being "basic", so it can only be done by a tedious process I'd rather avoid.

Thanks for the responses, this forum never fails!

 

[ringster]

I guess I am at somewhat of a loss as to the net gain of this discussion. Anyone else?

 

[ewh]

No net gain here

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[JLang17]

I don't know, I seem to have had my question answered so I'm happy.

 

[MechNorth]

Per 2.1.1.1 Positional Tolerancing Method. Preferably, tolerances on dimensions that locate featues of size are specified by the positional tolerancing method described in Section 5. In certain cases, such as locating irregular-shaped features, the profile tolerancing method describe in Section 6 may be used.

This lays out that the preferred method of locating features of size is the positional tolerance, and that profile of a surface may be used as the alternative. Where does it say anything about using +/- conventional tolerances to locate anything? If someone feels that 2.1.1(a) applies to the location of a feature of size, please back it up somewhere else in the standard with text or graphic.

This issue keeps coming up because the use of Preferably, Must, Shall, Should, May and other such terms is not widely understood within the context of legal documents. The terms do not have the same meaning as in conversational english. In this case, "preferably" is an indicator of the primary methodology, and establishes such methodology in a discrete statement. Acceptable alternatives are subsequently indicated in follow-up statements. It doesn't give you latitude to use any other method than what is listed.

Also consider that a "centerline" or "center" of a feature isn't physically present and reproducible without going back to the feature itself. Grab the axis of a hole! How are you going to find that hole's center repeatably? ASME addresses how to find the position of the center (axis or plane(s)) for features of size, but doesn't give any indication of methodology for verifying a +/- location. What about tying the feature's position to the datums? To invoke a datum reference you typically use a FCF. But +/- tolerances on location dimensions to the side of the workpiece are point-to-point, not center to datum. There's not one graphic or text anywhere in the book supporting the use of +/- location tolerances for features of size.
Off the soapbox now.


So, to the OP, if you're invoking Y14.5M-1994 or its ancestors, then you are bound to one of those two positioning methods. As you're not looking for a cylindrical tolerance zone, you can use separate "vertical" and "horizontal" position controls attached to the feature of size dimensions in each direction (vert & horiz); if the feature is cylindrical, then you can put them inline with "blank value" horizontal & vertical size dimensions respectively. In this case a position control of .010 vertically and .007 horizontally with the BASIC horizontal location shifted to the right (+ve) by .0025. You can't use unequal tolerance zones for position (i.e. +.006/-.001) controls.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[KENAT]

So, does that mean that this time you agree with me Jim;-).

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

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