What's your approach for tolerancing concentricity of a polygon, see attached image 2

[Perka]

I'm new to GD&T. What's your approach of tolerancing a polygon shape.

'Profile of a surface' as in option 1 locks down a lot.

At first I thought it looked down too much so I tried Method 2 using symmetry, which in the end pretty much did the same as profile of a surface.

Then I thought of some dotted inscribed reference circle with concentricity tolerance, along with parallellism tolerance.

Brain is confused to say the least. Suggestions?

 

[Hallec]

I would have to state the ubiquitous "Depends on the function of the part" first... Secondly, I would tell you that symmetry is rarely used in my experience, and Profile is much easier to understand, measure, and more easily captures design intent in most cases. Concentricity is interesting... Each of those methods looks theoretically sound, but would depend on function and/or the condition of the mating part. In the industries where I've practiced GD&T (firearms, Power, communications, defense, aerospace), profile of a surface would most likely be the default tolerance to use there.

EDIT: Also! Concentricity and symmetry have been removed from the 2018 standard, so there ya go... Was this a test?

I'm not a vegetarian because I dislike meat... I'm a vegetarian because I HATE PLANTS!!

 

[chez311]

Perka,

Here is a good discussion of control of polygon shapes and their use as datum features. Not sure if it is super helpful to your particular case, but definitely interesting (

https://www.eng-tips.com/viewthread.cfm?qid=446869).

As Hallec mentioned, profile would definitely be the first choice. I would avoid symmetry/concentricity at all costs for the same reasons that were mentioned - they are very rare except in very specific circumstances and are being phased out in the new release of the Y14.5 standard as a result. If profile results in a tolerance zone which is too tight - I am not 100% acquainted with the specifics yet as it just came out but the 2018* version has a new "dynamic profile" modifier that could be useful, which I believe works like a runout control for shapes other than those of revolution (ie: allows the tolerance zone to uniformly expand and contract). If the actual form tolerance of the profile can be tight, but location of the feature to the DRF can be loosened then multiple single segment profile or composite profile tolerance may be an option - keep in mind though that depending on the DOF constrained by your DRF some unintended consequences may arise (ie: if rotation is unconstrained - polygons with an increasing number of sides nears approximation of a circle and depending on the size of the tolerance zone/exact shape of the polygon the feature could rotate further than you might expect within its tolerance zone).

The shape could also be specified with directly toleranced (+/-) sides and angularity controls to a common DRF, or you could even do something like a wide profile tolerance and tighter angularity controls on each surface, however you have to keep in mind the variation allowed by these methods - the tolerance zone will not expand/contract uniformly.

*EDIT: oops - 2018 is the new standard, I'm a year ahead apparently (or behind, not sure which)

 

[Perka]

Thanks! Didn't know they were removed. That's ASME right? Couldn't find anything (free) concerning ISO so will have to lookup if it is removed there too.

Facet-to-Facet tolerance is the most critical form, maybe I can combine method 1 with a 60°±0.01 dimension for the polygon sides. Or might be bad practice since the cone shape of the polygon could be signifantly compared to the tight facet-to-facet angle tolerance. Need to take a courses in GD&T since this is on another level than what I've done previously.

I ran some numbers to for 'profile of a shape' tolerance and how it correlates to the facet-to-facet I want.

 

[chez311]

Facet-to-Facet tolerance is the most critical form, maybe I can combine method 1 with a 60°±0.01 dimension for the polygon sides

By method 1 do you mean the profile tolerance? Combining directly toleranced dimensions (whether angular or linear) to define the true profile for a profile tolerance is not allowed. You could do 6x individual profile tolerances but I would probably resort to a flatness tolerance since that is all it is controlling at that point.

Or might be bad practice since the cone shape of the polygon could be signifantly compared to the tight facet-to-facet angle tolerance.

Not sure what you're trying to say here.

 

[Sem_D220]

Method 1 looks like the best choice if you intend to control the form only. Since the all-around profile doesn't reference any datums, it will not control the size of the feature. If that is the intention, remove datum feature symbol A from the side view. Also, the angle should be basic.

Method 2 won't be well received from the reasons already mentioned in previous replies, but please note that it isn't applied correctly either: you need to derive datum A from some datum feature of width on the part, not from the 2 flats you control with reference to this same datum. Additionally, you need 3 datum center planes - one for each control.

Method 3 - as mentioned, just like symmetry, concentricity was removed from the latest ASME Y14.5 standard. If you follow the 2009 or previous revisions I think you can apply concentricity on a polygon (I've seen this shown in a book), but the control should be applied on the physical surfaces, not on the inscribed virtual cylinder. That is because the inspection involves deriving median points from physical surfaces. You will also need a datum axis derived from an actual datum feature. Do not connect the datum feature symbol to any center lines. The downsides of this method were also mentioned in previous replies.

 

[Perka]

Thanks for your great replies.

I have a new image with some corrections on the 3 methods. I will have a closer look at this when I get home.
I followed some advice here and put some basic dimensions and center lines in there.

Some questions in the image.

For example, center lines between opposing sides of polygon, good or bad practice?

 

[chez311]

Perka,

From your figure:
"does that mean all opposing sides (3x) are controlled by the profile of a surface all around 0.1?"
Yes. Any form deviation mus fall within a 0.1 wide tolerance zone equally disposed about the true profile defined by the 3x 40 and 6x 60deg basic dimensions.

To note, I don't think anyone suggested adding center lines - they can be useful depending on what you are doing, but in your case are extraneous, unless perhaps you are dimensioning to/from them. The inscribed circle in your method 3 is the one case they might be expected to be used though. What you need to remember is that datums are derived from,and controls are applied to, actual physical features - its a common error for example to define a width dimension and then attach a datum reference to the center line between that width because the desire is to define a datum center plane between this width, this is NOT allowed. The datum reference is applied to the width dimension/leader lines and by the rules in the standard it defines a center plane.

 

[Sem_D220]

Regarding the corrected image:
Method 1 - 40 and 60° are now basic dimensions. If you add "3X" before the 40 the whole shape will be fully defined with the basic dimensions and a profile tolerance. The size and form will be controlled. I should correct my previous reply and say - the reason the size was not controlled previously by the profile is that 40 wasn't basic, not because of the lack of datum references.

Method 2, 3 won't become viable as long as there are no datum features for symmetry and concentricity. The datum features for symmetry can't be the controlled features themselves, and the datum feature symbol for concentricity can't be attached to a centerline. Attached is a fragment from Dimensioning and Tolerancing Handbook by Paul J. Drake, Jr. (McGraw-Hill) that might help you specify concentricity correctly for an irregular symmetric feature.

Also, I would remove all the center lines you showed on the drawing. I think that the only cases were center lines should be shown are axes of surfaces of revolution or when you dimension location of features from center planes.

 

[Sem_D220]

One more thing - there is no purpose for the basic 60° in methods 2, 3. Symmetry and concentricity don't control orientation (edit: between the controlled feature and anything but the datum), and thus the angle remains uncontrolled without a direct tolerance.

 

[Perka]

Thanks Hallec, chez311 and SEM_D220. Lots of great response at this forum, glad I registered

Reason I added center lines on Method 2 was due to symmetry, but then I thought center lines might make method 1 easier to read as well, and wanted to hear your comments on it.

Did not know that '...the datum feature symbol for concentricity can't be attached to a centerline' (SEM_D220), might have some GD&T documents on my desk I should throw away, cause I'm pretty sure that they used centerline for concentricity datum, along with another example where the datum pointed at the dimension arrows, and said it had the same meaning.

Method 2:
Thanks SEM_D220, I read up on how to measure symmetry and realize that (like you said) two opposing side, where left side look like this ) and right side like this ( They would result in a "vertical line/zero assymetry" if you took some symmetry measurements with the caliper (measuring at different heights along vertical axis with the caliper jaws opening/measuring horizontally.
As suggested, remove basic from 60° dimension

I'd also need to add parallelism to control the form. And from what I've read tonight I have to have the datum feature on a surface (instead of axis) if I want to control form with parallelism, in other words surface parallelism. On the image it was pointing at the 40 dimension arrow (axis in the center of polygon), which would not be correct in this case I believe (lots to learn). Need to figure out if I need surface parallelism or flatness on the faces... hmmm.

Back to symmetry for method 2, how would one go about placing a symmetry datum, is it possible given I only have "one shape/feature, extruded polygon"?

The datum features for symmetry can't be the controlled features themselves, ...

*edited Good quote that I will try to remember from now on

What you need to remember is that datums are derived from,and controls are applied to, actual physical features - its a common error for example to define a width dimension and then attach a datum reference to the center line between that width because the desire is to define a datum center plane between this width, this is NOT allowed. The datum reference is applied to the width dimension/leader lines and by the rules in the standard it defines a center plane.

 

[3DDave]

It seems like another case where the OP hasn't got copies of the ASME standards. I understand the politics of the cost, but it's a shame that it costs so much. Whether it's "worth" that amount is debatable.

In ASME Y14.5.1-1994, there is support for 6-way symmetry. It's not limited to planar mirror conditions. It's still described that way in the current draft.

 

[Sem_D220]

Peka,
Glad you found our responses helpful. I have to say that the credit for your last quote belongs to chez311, not to me

Before you throw away the GD&T documents on your desk, make sure you know which standard your company is supposed to work by. I know very few about the ISO GD&T standards - only what I read online in and in this forum, but I'm sure I read somewhere that they allow attaching datum feature symbols to center lines. There are members in this forum who can confirm or deny this.
If ISO allows this, I don't know if there are any specific conditions for it, but it sounds to me like a bad idea regardless of being allowed or not. For a part that has 2 or more coaxial diameters or 2 or more symmetric widths, if the datum feature symbol is attached to a center line that goes through the entire part, no one will know which feature is the datum feature that must be used for holding the part in the inspection fixture and for simulation of the datum axis or center plane.

As for surface parallelism, its main purpose is to control orientation, but it does control form (flatness) as a side effect. Parallelism and the other orientation controls can also apply to a feature of size rather than to a surface, and in this case, it is correct to align relate the parallelism feature control frame with the dimension line (adjacent to an arrow or replacing one)., by placing the feature control frame under the dimension of width or diameter (sorry for the corrections, some concepts got mixed up in my head when I wrote that), The controlled element, in this case, is the center plane that should be derived from the feature which is dimensioned and toleranced.

 

[pmarc]

Thanks! Didn't know they were removed. That's ASME right? Couldn't find anything (free) concerning ISO so will have to lookup if it is removed there too.

It is more like another case where some advice is being given based on ASME while it seems like it is the ISO that should be brought to the table in the first place. OP should know that both systems have their own sets of rules, concepts and modifiers.

 

[Perka]

I raised the question about which standard we work on (recently hired)
I need a center hole through the part and thought this might be a good way to control the geometry. The hole sets the datum A which is then referenced for symmetry, perpendicularity and parallelism in different view orientations (which may imply I need to have a new datum feature for each new view?)

If symmetry is allowed in the standard we work with, do you see anything being overdefined/conflicting/missing with this method?

I see a potential mistake, perpendicularity would only be needed in one view?

 

[Sem_D220]

Perka, the datum derived from the hole is an axis, not a plane. All parallelism controls and the 2 perpendicularity controls can reference this datum. You can do that by simply adding "6X" before the parallelism control if the paralleliam control should be applied to each of the 6 flats. Make sure that the hole is a functional datum (what role does the hole play for this part?). By the way, I added a small correction to my reply above, make sure you noticed it and sorry if it was confusing.

 

[Perka]

The hole axis is the axis that the polygon need to be concentric about.

Thanks for clearing up the datum reference feature.
Flatness in combination with parallelism does not seem to be controlled on my drawing?
Parallelism is measured over the whole surface but the angle does not control the shape of a polygon face, right? Perhaps make 60° a basic dimension and add angularity tolerance(s).
^scratch that (if the angle at some point on the surface were to be much larger than 60°, the shape of the face wouldn't pass the parallelism tolerance)

Here is the progress so far

 

[3DDave]

I'd suggest buying a copy of the applicable standards for the place where you work. Otherwise it will be a game of 2000 questions.

I'm more curious about the stress analysis that's used to determine the tolerances and the need for symmetry.

 

[Sem_D220]

if the angle at some point on the surface were to be much larger than 60°, the shape of the face wouldn't pass the parallelism tolerance

The parallelism tolerance does not control the 60 degrees angle. That angle is controlled by the direct +-0.1° in your drawing. Since you control each facet with reference to an axis, each facet can rotate about that axis to any orientation and still be parallel, hence no mutual orientation is controlled by parallelism. 6X can be above the feature control frame, not an issue. 3X should stay as it is and the feature control frame for symmetry should be placed under the dimension. Not sure about the two leaders that originate from a single perpendicularity control. All these are just technical tips, but you are strongly advised to consider the Profile scheme again. You could reference the datum axis at Profile and achieve the desired orientation of the external surfaces with reference to the datum axis. You are also advised to consider replacing symmetry with Position. Position is much easier control to inspect, and if the prime goal is centering of features, it is considered the preferred one.

 

[chez311]

I raised the question about which standard we work on (recently hired)

pmarc - sounds like OP is unsure as well, you are correct that should have been our first step to determine.

Perka,

As pmarc noted the standards can differ in their treatment of datum definition and controls/modifiers. You should definitely determine what standard you should be working to before proceeding much further.

Just to build off of what was mentioned by Sem, I too have limited knowledge of the rules surrounding the ISO rules for datum definition but there is a good reason why the ASME spec does not allow attaching datums to theoretical centerlines/axes/points. In addition to my (and others) previous comments about those theoretical features being derived from physical features - Sem's comment about ambiguity is another driving factor. See the below figure - without attaching it to a specific width it is impossible to determine which feature the datum is derived from (multiple widths or hole?) and what exactly the datum looks like (centerplane or axis?).

This was drawn from a comment by JP back in 2011 from this (

https://www.eng-tips.com/viewthread.cfm?qid=292841)

thread - all credit goes to him, I hope he doesn't mind my referencing it. Theres some good posts there about the ASME rules regarding datum definition/specification, however your best friend would be again to determine which standard applies in your workplace, and read through the applicable sections - theres no better reference than the primary source.