GD&T machined octagon centered on shaft 6

[MechTech2000]

Lets see if you guys can figure this one out,
I'm correcting old designs and drawings for my company, and I'm trying to clearly indicate the concentricity of an octagon shape on a shaft.
This octagon is to be press fit into a pinion (68mm h6).
Datum [A] is the center of the shaft.
The ground cylinders that will mate with bearings are: '[CON|Ø0.030|A]'.

I've looked at using basic dimensions: [3x45.00°] & [SYM|0.000(M)|A] except that symetry does not allow the of MMC.

Do I have to use profile tolerance for this application?

 

[ewh]

"Concentricity is is a condition of a surface of revolution in which all points of the surface are equidistant from a common axis."
An octogon does not meet these conditions. Profile may be the best alternative.

 

[Heckler]

The application of concentricity is complex and rare. I would consider uses position, runout or profile before concentricity but in your case I would use profile.

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 5.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NVIDIA Quadro FX 1400
o
_`\(,_
(_)/ (_)

Never argue with an idiot. They'll bring you down to their level and beat you with experience every time.

 

[ctopher]

I agree with Heckler. I very rarely used concentricity. It is more difficult to inspect.

Chris
Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 06-21-06)

 

[CheckerRon]

Amen to profile. It is the way to go for this application.

 

[MechNorth]

My preference would also be to use Profile of a Surface. There is another alternative, however.

You can use positional tolerace to locate the center plane of opposing faces because they are features-of-size. This also allows you to use MMC if appropriate.

Jim Sykes, P.Eng, GDTP-S
Profile Services
CAD-Documentation-GD&T-Product Development

http://www.profileservices.ca

 

[namdac]

I as well agreewith heckler. I would go get the Octogonal material from stock, check Central Steel and Wire catalog. This is a stock item.
Regards,
Namdac

 

[MechTech2000]

Getting closer?




Solid Edge v7 to v19
Dell Precsion 370
2GB DDR2
WD Raptor 74GB 10k (OS+Programs)
2xWD Raptor 74GB 10k (Swap+temp)
nVIDIA QuadroFX3400
2x 19in LCD
3DConnexion SpaceBall 5000 USB

 

[dingy2]

Cylindricty and the 2 runouts are applicable on round features of size - not applicable here.

The profile of a surface is theoretically applicable since it would control the shape and location relative to the datum but one must have a CMM with scan mode to measure this feature. It would not be measured on the shop floor well unless this equipment is available.

Positonal tolerances may be the best approach and one could use MMC. I would suggest a 0 tolerance beyond MMC since this hex shape has a snug assembly fit. I would also reference my datum(OD) at MMC. I might even place the word "BOUNDARY" below this FCF. The virtual condition is actual the MMC size and shape of the hex.

This would then be conducive to a checking fixture in which there would be a hole of MMC size for the datum and hex at the MMC size and in true position to the datum. One would then place the part datum first into the fixture and rotate the part so that the hex lines up. The part should then be able to be pushed (with the force of 1 finger) all the way down in the fixture. If it goes all the way, presto, the feature is within tolerances.

This feature could then be confirmed on the shop floor by the Operator.

Dave D.

 

[MechNorth]

MechTech, getting there, but not done yet. Pls click on the following link for how I'd tackle this, at least at first glance.

http://www.profileservices.ca/files/tidbits/tidbits_missc.html

Symmetry & Concentricity are too hard to validate, so don't use them ... EVER! You don't need the 45-degree angles to be shown; they're quite obvious from the graphic. The toleranced size across the flats shouldn't be used if you're using the surface profile to control the flats. The radius shouldn't be reference, it should be basic. The profile tolerance should be .05-ish with a unilateral-inside zone (shown by a heavy chain line inside of the geometry). You can / should use positional tolerance to locate the center plane generated by the dimension across the two edge radii. There isn't much contact area on those radiused edges at the vertices of the octagon, so they're not really a good locating surface. They would be better if the vertices were rounded by a Dia-36.5 cylindrical surface, with reduced flats, providing that the alignment within the pinion is more relevant than the secondary use of the flats.

Make any sense, MechTech?

Dave, verification of the surface profile on the flats is extremely easy without a CMM. Chuck the workpiece on the feature of size that is generating the datum axis; chuck should be inspection quality and indexable. Lock the workpiece from rotating once a flat is in a horizontal position. Zero an indicator at the basic offset of 34 from the axis of the chuck, and check for deviation from there. Rotate the workpiece basic 45-degrees, and repeat the check. The controlled alignment diameter can also be checked in the same setup. It's a very quick method, and yields numeric results rather than go/no-go.
The gage you describe would also work nicely, it's a question of quantities and the need for numeric feedback. It's always nice to have options.

Jim Sykes, P.Eng, GDTP-S
Profile Services
CAD-Documentation-GD&T-Product Development

http://www.profileservices.ca

 

[drawoh]

MechTech2000,

I looked at your drawing.

If your octagon is being pressed into a mating octagon shape, your tolerancing should be very simple, albeit, very accurate. Just use a profile tolerance all around. The symmetry and the +/- tolerances do not help you. Your drawing defines the distance between opposite faces very accurately, but allows adjacent faces very much more error.

If it were my drawing, the surface tolerance would be 0.01 all around, and I would use a phantom line to show that this error all went inside from nominal. See Figure 6-15 in ASME Y14.5M-1994. I would not bother with the point to point dimension except maybe as a reference. I would specify the radius sloppily as something like +0.5/-0.

JHG

 

[gpavlab]

If you wanted to try using concentricity in this case don't do it directly with your polygon, instead use an inscribed circle in the polygon. That should eliminate some of your problems in displaying positional and relational feature controls.

 

[dingy2]

MechNorth - I do agree with you on the method of measuring Profile of a Surface on hex surface. One must make sure that the initial face must be level rotationally and then after that surface is confirmed, rotate the part 45 degrees and go again. One has a +/- .005 using a profile tolerance of .010.

If one goes in this direction, make sure that there is only a small number of parts being produced and all dimensions reflecting the angle and distance would be basic. One does not need the point to point dimensions, only the flats and the angle.

Position at MMC is appropriate for large number of product.

 

[powerhound]

I was always under the impression that concentricity controlled centerlines between features regardless of the shape of the feature therefore you could call out a round shaft concentric to the end of a square bar or vice-versa. I would have recommended calling the profile of the hex concentric to the shaft, however seeing as most others here seem to be settled on "profile of a surface" I'll have to re-evaluate my understanding of the concentricity callout.

Powerhound
Production Supervisor
Inventor 11
Mastercam X
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[ringman]

MechNorth,

I have read many of your responses and agree and am generally impressed with your knowledge of GD and T.
This particular thread is perhaps with more than one good solution however.

I tried unsuccessfully to open your link to your proposed solution. (I am by no means a computer 'whiz'.) So I am left without the solution that you proposed for this.
If there is another way to get it please let me know, thanks.

But I still am left with one question, regarding the statement that you made that the 45 degree angle was obvious. I thought it looked more like a 44 degree angle. Which is to say that I think it needs to be specified.


What do you think?

 

[MechNorth]

Ringman, thank you for the compliment.

I don't like to post things on third-party sites, but if you reach me through my website, I'll send you a PDF of the graphic.

The 45-degrees is from basic geometric relationships of regular polygons and complementary angles. I've posted the graphic explanation, but it's basically the same as from Machinery's Handbook. I started to type out the explanation, but that made it look very complicated. I'll send it with the dimensioning graphic also.

http://www.profileservices.ca/files/tidbits/tidbits_missc.html

Jim Sykes, P.Eng, GDTP-S
Profile Services
CAD-Documentation-GD&T-Product Development

http://www.profileservices.ca

 

[ewh]

powerhound,
The quote I posted defining concentricity on 24Oct06 is taken directly from ASME Y14.5-1994.

 

[powerhound]

ewh,
I went back to the source that I originally drew that conclusion from and I'm not sure what to make of it. It's on the tec-ease.com website and it's one of the GD&T tips of the month. Look at runout vs. concentricity and see what you think. I may have taken the article out of context. I deal with this callout unnecessarily on almost a weekly basis as people think that concentricity is always the best way to call out concentric features. We do a lot of large tubes here and because tubes are cylindrical in form, everybody calls out cylindricity when it's absolutely unnecessary. I guess it's just something you have to deal with when most draftsmen have only basic GD&T familiarization training and then they're turned loose.
If you go to the site I talked about, let me know your thoughts. I'm always on the lookout for new views and challenges. That's why I like this place so much.

Powerhound
Production Supervisor
Inventor 11
Mastercam X
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[MechNorth]

Concentricity is one of the most commonly misunderstood and hence misused controls that I've seen (Symmetry is another one). The most common misconceptions are that (i) concentricity relates to two surfaces which follow each other without respect to a center point or plane, and (ii) concentricity only applies to a nominally circular surface. Sometimes you have to study & re-study the standard to get the subtleties, and this is one of those times.

Under Y14.5M-1994, 5.12-Concentricity: "Concentricity is that condition where the median points of all diametrically opposed elements of a figure of revolution (or correspondingly-located elements of two or more radially-disposed features) are congruent with the axis (or center point) of a datum feature.", which means that it is not restricted to nominally circular features, but rather to elements of opposed features (i.e. on opposite sides of a center point or center plane), as indicated in some illustrations in the Tec-Ease tip.

5.12.1, last 3 lines of the first paragraph; "...a concentricity tolerance requires the establishment and verification of the feature's median points."
5.12.1, Italicized paragraph; "...finding the median points of the feature may entail a time-consuming analysis of surface variations. Therefore, unless there is a definite need for the control of the feature's median points, it is recommended that a control be specified in terms of a runout tolerance or a position tolerance." ... in other words, don't do it!!!

The Tec-Ease Tip illustrates several configurations where concentricity can but should not be used, and illustrates that in the particular case of round features, total runout should be used instead. Unfortunately it doesn't show the preferred controls for the other situations. I'll drop a note to Don @ Tec-Ease to see if he can amend that Tip.

Jim Sykes, P.Eng, GDTP-S
Profile Services
CAD-Documentation-GD&T-Product Development

http://www.profileservices.ca

 

[powerhound]

Thanks Jim,
I feel a little better now. I always broke concentricity down to this: It only controls centerlines; The form of the features will be controlled by the tolerance unless another form control is applied. From your reply, I think I was correct in my understanding of concentricity and although concentricity is usually reserved for high speed (RPM) applications and such, this might be an exception considering it's not as difficult to check because there are flat surfaces to measure from. The biggest problem I can see is that the flat-to-flat tolerance (opposing flats) may have to be unnecessarily tight to keep the hex looking symmetrical. I guess when that is taken into consideration, profile of a surface may be the way to go here. What do you think?

Powerhound
Production Supervisor
Inventor 11
Mastercam X
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II