Re-tolerancing a Lug Pattern for Hard Gauging

[Udja]

Hello all,
I am currently trying to re-do one of our drawings with the intent of being able to hard gauge the parts during our QA. The issue is that I just don't have a firm enough grasp on GD&T to do this right, and trying to apply what I've researched is making me even more confused. So, I figured I would just see if I could ask for help.

I've attached a sketch of the section in question; it's an 8 lug pattern that is clocked 22.5 degrees from the vertical plane. ASME Y14.5M-2009 is how it's to be interpreted and it's what I've been muddling through all day. -A- through -C- are established in other drawing views on other features, but I've tried to include them to help clarify things. -A- is based off the outside diameter, -B- is parallel to the plane of the drawing view, and -C- is a vertical plane that runs through the cylinder's axis.

Again, I'm trying to get this part to where we could hard gauge the lug pattern. I've been told that the best way to do this is to use a profile tolerance, but I'm just not familiar enough with GD&T to be able to do this confidently. The drawing view attached is my best attempt. How bad is it?

Specific questions:

- Am I going about this wrong by even attempting to put a surface profile tolerance on a pattern? Again, I've never had to use much GD&T, so much of this is foreign to me. My only other thought was to simply use a surface profile on one lug and then just say "pattern 8 times equally spaced" but I felt like that left things too open-ended. On the other hand, applying a profile tolerance on the whole pattern made it so that I had to make every dimension on the part basic as each dimension will be used in the pattern...which just seems like overkill. How should this be done, if I'm off-track with both of my trains of thought?

- I've used a position tolerance on the .191 dimension.(Edit: It seems the file I uploaded actually has the surface profile symbol in the tolerance box, which is an error on my part. It's supposed to be a position symbol) This dimension and the 16 degree angle control the size of the slots; does that make the .191 a feature of size? As best I can tell, I think so, so I've used the position tolerance. Should I have used a surface profile instead? Or should it be toleranced without GD&T, with just a symmetric tolerance zone? If that changes, does the 22.5 degree dimension then become non-basic, or should it stay basic because of the profile tolerance around the whole pattern? And I don't even know what the 16 deg should be toleranced as, so I've completely guessed on that one.

- Our old dimension scheme had the two diameters on the left of the drawing view dimensioned as bilateral with +.003/-0. The inside, radial edges of the lugs, however, were toleranced symmetrically. I'd like to mimic that but I'm not sure how to go about it. I could simply change the actual part dimensions so that the diameters 'split' the old tolerance zone, but I feel like I've seen a way to call out specific sections of a surface profile as unilateral without effecting other sections of the profile.

I realize that I've asked a lot of questions, and I appreciate any help I can get. This is the first time I've actually had to ask for help because the archive of questions here is simply astounding; I can usually find what I need just by searching. I'm at a loss on this one, though, so thank you again for any help!

 

[ewh]

Welcome to the site!

The first thing that jumps out at me is datum C; is it an arbitrary theoretical plane, or is it defined by a feature? If following Y14.5, it needs to be derived from a feature.
Per ¶4.8 "A datum feature is selected on the basis of its functional relationship to the toleranced feature and the requirements of the design... Datum features must be readily discernible on the part." A theoretical plane not associated to a feature would not be readily discernable and would not be correct.

Also, the callout for datum C violates the standard. Per ¶4.8.2 "... The datum feature symbol identifies physical features and shall not be applied to center lines, center planes, or axes."

Profile is a good control for what you are trying to accomplish. Using all basic dimensions to define it would not be overkill.

I'm sure other, more knowledgeable members will help further.

"Know the rules well, so you can break them effectively."
-Dalai Lama XIV

 

[drawoh]

Udja,

I agree with ewh. Datum[ ]C must be a feature. Can you drill a hole or apply a flat somewhere to provide an unambiguous clocking feature?

By "hard gauging", you mean a go-nogo gauge, right?

A crude rule of thumb is that a go[ ]gauge tests all of your features. A nogo[ ]gauge tests one feature, only. If your .003[ ]profile is valid all around, you can construct a go[ ]gauge. You make no-go[ ]gauges to test the internal Ø.687 and Ø.935[ ]dimensions. Yet another gauge can test your 16[°] face at your pitch circle.

As far as your drawing is concerned, a .003[ ]profile all around, is inspectable, especially with a go[ ]gauge.

--
JHG

 

[3DDave]

Answer 1: If the surfaces of the feature work in concert then they can share a tolerance, such as the profile all-around would do. The callout in the lower right section is pretty good, except for needing an all-around symbol.

The application of a profile to a basic dimension ([.191]) is not typical and doesn't appear to control the related surface as it is indicated as two intersection points. More typically one would indicate two locations on the profile and then point at the part outline between the points and use the Between symbol to show that the profile tolerance applies between the two indicated points. You would also use the '8X Individually' to indicate the same references apply multiple times; 8 in this case.

Answer 2: If you intended to use position on each tapered feature then I think that's a mistake. Tapers aren't features of size. The reason being that no matter what value you assign to their local size they will meet that value somewhere, and there's no inherent direction associated with a change in angle. You might use symmetry relative to [A] to tighten the centering. You might use straightness of line or angularity to make sure the lugs surfaces are parallel to each other or to the center of [A].

Other discussion:

[A] fixes two rotations and two translations; [C] may do clocking depending on what feature is selected as a reference; this leaves with nothing to do in the [A|B|C] frame of reference because there is no axial component being controlled in the section.

I don't know what improvement you might make in mating with another part except to use a smaller profile tolerance with respect to A. You can use position applied to the entire boundary, but that won't really make the fit better. It would be used to allow the feature to float more than the profile tolerance allows.

You might also create a smaller profile tolerance applied to each lug individually to improve form control, but that won't improve the overall fit.

Finally, when you get a chance, you will find "GD&T" is neither defined nor described in any version of the ASME/ANSI Y14.5 standard. It hasn't been in there going back to 1982. At best one can either use or not use feature control frames with geometric characteristic symbols, abbreviated as "FCF"s, as in should I control this with FCFs? Taking it as marketing-speak, GD&T applies just as much to conventional dimensioning and tolerancing without using FCFs.

 

[Udja]

Thank you all for the welcome and the feedback!

First, to ewh and drawoh, datum -C- is indeed established by a feature on the part; it's not arbitrary. I included it on the image I provided to try to bring clarity to what I was trying to reference...it is generated by a hole drilled top dead center of the part further along the part's axis. It's called out properly in another drawing view.

Drawoh: yes, go/no-go gauges are what I'm trying to get to. We've got a gauge to check the clocking of an individual lug, but we've run into issues with vendors single point broaching the pattern (our 'good' vendors will use a custom broach to cut the whole pattern at once) and it has become more crucial to be able to check the whole pattern at once. We currently have to send these parts to our second location across town to be run on a CMM if we want reasonablyquick, accurate reports on the pattern profile.

3DDave: Thanks for correcting me on the FCF and GDT thing; I've been fortunate in that I've been part of one Engineering department since I graduated a few years back, but that means if nobody refers to something technical by its proper nomenclature, I carry on in blissful ignorance. 'Fitment' is another one that gets tossed around here to describe how well parts fit together, but the actual definition of that word and how it gets used around here are comically different.

Features working in concert being able to share the same tolerance makes sense, thanks for that explanation. I'll add the all-around symbol as well.

Thanks for explaining why tapers are not features of size, even if dimensioned as I did. Like I said, I was having trouble thinking through why it is or is not a feature of size.

Is there simply a better/more concise way to define the angle and size of the lugs without using a pair of intersection points on a reference circle like I've done (maybe use the VS from the .935 or .687 diameters)? If the cutout was not tapered, I believe I could just give the slot a position tolerance referencing A and C, but the 16 degree angle on the slot is giving me trouble. If I'm reading your comment correctly, it would be better to replace my (intended) position tolerance on the basic .192 with a profile tolerance from two points on either side of the cutout? I've attached an updated image to clarify that last sentence. Is it acceptable to use the basic dimensions only and remove any FCF's from the slot entirely?

 

[tbuelna]

What you are dimensioning/tolerancing is a form of straight sided internal spline. Take a look at MIL-HDBK-400, figure 109.

 

[3DDave]

The ends of the limited profile would be at the ends of the contact surfaces, rather than from mid-point to mid-point.

It doesn't really help the fit unless the mating teeth are free to move individually.

The symbol you have there is profile of line, which only applies to individual levels. Think of it like a deck of cards. Each card has a precise line profile, but you can fan the deck. In your case the line control is on each card, but the all-around profile is what controls the shape of the deck.

If the mating part only contacts the faces of the teeth you can use the <--> symbol and leaders and notes to indicate the extent of the face that will be controlled and use

[profile|.003|A] 16 PLACES X <--> Y.

The same technique could be used to cover the root and tip profile tolerances but with a different size of tolerance zone.

Since they use the same DRF, ([A]), they should apply simultaneously, though adding SIM REQT would help nail down any doubts. Then you fixture is one that is at the least material boundary of the profile and is MMC profile is checked by using feeler gauges that are the same as the profile tolerance size. If the GO gage fits and there isn't enough extra room for the feeler guages (flat or round pins) then the part is good.

As a practical matter I'm not sure that .003 on this small part will work so well, but that's the theory for how it could work. Another option is using zero expansion metal to cast the bore of the part and using that in an LMC boundary GO gauge.

 

[notats]

I cant help noticing that the profile FCF references a fictious -B- on the attached drawing that probably is the -y- axis C/L ambiguous theoretical plane like -C- is. I didnt see it mentioned in the previous reply posts.