Geometric Dimensioning and Tolerancing 1

[mm2c]

mm2c (Mechanical) 13 Mar 05 20:07

can anyone explain the proper use of
PROFILE when the part is dimensioned using +/-
tolerances instead of BASIC dimensions?

 

[ewh]

The surface to which the profile is being applied may be located by +/- dimensioning, but the elements making up the surface must be dimensioned with basic dimensions.

 

[drawoh]

mm2c,

All the tolerances applied to the part must be satisified by the fabricator. Any features that satisifie the most accurate tolerance ought to satisfy the less accurate ones.

The only problem with this is that you might have a control that allows the feature only to exceed the nominal material condition, and another control that allows the features only to be inside the nominal material condition. This is a mistake, and you will have to fix it.

Consider the case that you have a part with an elaborate outline to which you have applied a profile tolerance of 0.5mm. You apply the all-around symbol. You apply basic dimensions all around with one exception. To that, you apply a tolerance of +/-0.1mm. You could just as easily have applied a tighter profile, but the +/- tolerance could be exactly what you need.

Any feature falling within the +/-0.1mm feature also falls within the 0.4mm profile. The part can be inspected. The drawing is valid.

There is a way to apply a profile tolerance to all the features except your accurate one, but it is slightly complicated. If you have more than one accurate feature, it is a lot more complicated.

The whole point of basic dimensions is that you are indicating that the feature is controlled by a geometric specification. You should use basic dimensions unless you need an additional control.

JHG

 

[type26owner]

Profile is only used in conjunction with basic dimensions. Locating surfaces using +/- tolerances are subject to Rule #1 in the USA. Rule #1 called the Taylor Principle states that size at the Maximum Material Condition also controls the form. That's okay for simple relationships as long as an origin symbol is ALWAYS used. Never stack or sting together +/- locating dimensions or the indirect tolerancing method becomes a problem. GD&T is best utilized when only direct tolerancing is the applied.

 

[PaulJackson]

Paragraph 6.5.5 of the ASME Y14.5M-1994 Standard and figure 6-18 support the response from EWH. If you read the section on profile it may help you to decipher how the tolerance zone is applied or if it is improperly defined.

 

[looslib]

You can NOT use +/- tolerancing with profile.
All dimensions MUST be basic for the outside profile.

We just started a GD&T training class this morning and the instructor emphasised this point.


"Wildfires are dangerous, hard to control, and economically catastrophic."
"Fixed in the next release" should replace "Product First" as the PTC slogan.

Ben Loosli
CAD/CAM System Analyst
Ingersoll-Rand

 

[Heckler]

The profile of a line and surface must be defined by basic dimensions.

Best Regards,

Heckler

Do you trust your intuition or go with the flow?

 

[ewh]

Ben,
According to the standard, you can use +/- dimensions to locate the profile. The profile itself must be dimensioned with basic dimensions. Ask your instructor about paragraph 6.5.5 and figure 6-18 (as pointed out by PaulJackson).

 

[ajack1]

I am not sure what is used in the USA but certainly in Europe at least in the automotive industry JIS B 0025 is the standard.

Most automotive parts now have very little conventional dimensions on them partially due to the fact that the shapes are so complex it would be impossible.

So parts are toleranced from a model. A profile is like a flat “C” at -90 degrees and should be followed by a size say 0,5, a surface is like a flat “D” at 90 degrees and again is followed by a tolerance.

This denotes the diameter of a circle or sphere that runs along the true model and the part must be within this.

So to this standard there are no +/ - dimensions as such, however you can have only – dimensions by making the tolerance unilateral, in which case the whole tolerance is on one side only.

 

[type26owner]

Profile is the highest level defining control that exists. It can control location, orientation and form. Figure 6-18 just illustrates one of the special derivations of profile which is used in this case to control only orientation and form and not location. It can be used to control just the form also. Only if it's meant to be a one of a couple of special situation controls would there no basic dimensions. Like for flatness. 90 degree basic angles are also permitted to be assumed without being specified as such so it could be used as perpendicularity too. There might be others also that don't come flashing back in my memory at the moment also.

If you reread the original posting it says 'instead'. That means to me there aren't any basic dimensions.