Position each of the three pairs of parallel faces to the axis or, preferably, use a profile tolerance to control the variation in form and location.

@3DDave thanks for your response! I have just one question though, is one method superior to the other in terms of cost saving? (i.e., is it easy for the machinists to do the profile?)

If the machinist is using a rotary broach, then it probably is. It depends on the machinist.

See http://www.polygonsolutions.com/how-rotary-broachi... for an example. There are other suppliers; Google search put this one at the top of my list.

Other than that, the callout is really so the inspector can verify that the part meets requirements and for the engineer to accurately record a solution to the problem. If the solution requires uniformity of shape and that shape needs to be located in some way, then profile is a correct choice.

Great, that clears up a lot thanks again Dave!

Another solution could be:
Directly toleranced size hex dimension, phantom maximum inscribed circle around the inside hex and position associated with it. Position could be at MMC to help functional gaging for assembleability.
True profile of the inside hex would be dimensioned with basic angles and basic corner radii.

I got this concept from another discussion where pmarc participated and I would like to know if can be applied here. All the credit ( if solution is acceptable) shall go to pmarc.

Of course the OP has to use 2009 versiun of ASME Y14.5 so the position callout can be applied to irregular features of size.

No one else is concerned that the 5/8 threads are the primary datum?

Well, if the thread is doing the job of orienting this part in the assembly, probably is a good choice to be a primary datum.
What else COULD orient this part? How this part physically interacts with its mating components in the assembly? Physical realities of this assembly.

Just was surprised that no one mentioned it. Every GD&T author that I have read says to never use threads as datums unless you absolutely have to. That sentence is usually followed up with one that says even if you have nothing else to choose from you should still consider not using them.

greenimi,
This solution would be the last I would use and recommend in this case, unless there is really a functional need to define something working along dynamic-profile-tolerance-zone lines. The reason I came up with this method was that in the 2009 version of the standard there is no tool that would work similarly to "dynamic tolerance zone" modifier (as proposed in the new draft of Y14.5). The tricky part of it is that hex contour is not fully defined with basic dimensions, and so many people may see this as a violation of the profile tolerance application rules. I personally think it is more like extension of principles (supported by the infamous figures from the standard where cones are controlled by combination of directly toleranced +/- diameter and profile tolerance).

With that said there are at least couple other ways to control hex features, and most likely at least one of them will grasp the design intent (some of them have been already mentioned):
1.Three position feature control frames applied to each pair of parallel faces and referencing to A. Tricky part of it: inspection will have to know that these position callouts apply simultaneously, so in fact the angles between center planes of pairs of faces are also indirectly controlled.
2. Simple all-around profile callout wrt A.
3. Composite all-around profile callout with upper segment referencing A (location control) and lower segment with or without A (size/form, or size/form/orientation control).
4. Combination of datumless all-around profile tolerance and position at MMC.
5. Combination of datumless all-around profile tolerance applied directly to hex contour and position at MMC wrt A applied to a phantom maximum inscribed circle.
6. A little bit more tricky application of combination of datumless all-around profile tolerance applied directly to hex contour and position at RFS wrt A applied to a phantom maximum inscribed circle.

These are all great answers guys, thanks!
All these make sense to me however I am relatively new to GD&T, how would you carry out number three? Would it be like in this picture?

And if it is like in the picture does it essentially mean that the bottom part provides a hexagonal shaped tolerance zone of 0.02 (constraining the actual profile of the hex) and then the top part provides a 0.05 tolerance zone (also hexagonal) in which that pattern must fit?

Thanks again!

• http://files.engineering.com/getfile.aspx?folder=9a94734f-83ad-42f6-886f-3a

Great post and discussion. Note: The distance across the flats needs to be BASIC.

Certified Sr. GD&T Professional

Regarding the use of threaded features as a datum - meh... they make Jo Plugs for a reason. There are occasions where a threaded feature is actually serving more functions than simply fastening, but I absolutely agree that it should be treated as exceptional. http://www.judgetool.com/tappedholelocationgages.a...

You'd be hard pressed to prove your case if the thread in question was something like a 1/2-13 UNC-1A though...

The distance across flats indeed needs to be basic.

As for the datum threaded feature, from what I see on the original drawing datum axis is derived from thread major diameter, thus datum feature simulator is contractable cylindrer, not thread.

Well, I think you know how to call profile out properly and don't forget to add the "all around" symbol on the polygon.

Season

• http://files.engineering.com/getfile.aspx?folder=e2cf964b-a01a-4629-abfe-39

Sweet, thanks again everyone this was seriously helpful!

Thread-as-datum doesn't concern me much at all if it's on the major diameter.. that feature is easy to control well and easy to gage.

For /external/ threads, sure. Easy to control, easy to gage, and almost useless as a functional feature. So not a very smart choice in most applications.

But a perfectly functional one in certain instances, which is the point I was making.