Looking for an inspection method for this true position callout

[Iceman13]

Good morning,

I am looking for an acceptable method of checking the true position callout on a part we are manufacturing WITHOUT the use of a CMM. My idea is to use a pin micrometer to check the locations of the slots in this part at 6 places around the OD. I am wondering if this inspection method would suffice even though we would be checking TIR in my opinion by doing so. The OD on these parts always runs true to the Datum -B- ID within .0001".

Also, would the limit of variation measured be a total amount then of .002" or .004". To be honest I am wondering as well if this print is even properly called out as the diameter symbol is not included in the feature control frame, which seems unusual to me being that this is a circular part.

Thanks for looking and all responses and ideas are appreciated.

 

[djhurayt]

Need to think more about the "how to" part. But with regard to the tolerance zone, the lack of a diameter symbols results in a square tolerance zone that can vary in the X+, X-, Y+, & Y- by 0.002". So your tolerance zone is actually a 0.004" square as opposed to a 0.002" diameter circle if the diameter symbol was included in front of the .002 in your FCR.

david

 

[axym]

Iceman13,

I'm not sure what to suggest here. The drawing appears to be done by someone who does not have a good understanding of GD&T per the standards, and therefore has a lot of "specification uncertainty".

First, the position callout is not standard compliant. The feature controlled by the position tolerance appears to be an imaginary circle best-fit circle that goes through all 36 slots. It is not legal to specify position on such a circle, and there would be no way to uniquely define the circle on a real part.

The intent seems to be that the "circle of slots" be concentric with the datum -B- ID. They probably want the radial location of each slot center to be accurate and consistent. But these are guesses - the drawing doesn't clearly indicate these things in a way that can be objectively verified. So you will need to either get a clarification from the customer or come up with an inspection method that you feel verifies the perceived requirements. The suggested method of checking the distances between the slots and the OD seems reasonable - if these distances are consistent and the size of the slots is accurate, then it is likely that the radial location of the slots is accurate.

Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca

 

[dgallup]

That is a completely bogus position callout and therefore there can be no correct way to inspect it.

----------------------------------------

The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.

 

[powerhound]

Yeah, like dgallup said with no sugar coating. This is a bad callout so anything you come up with is only going to be random numbers that don't matter a bit.

John Acosta, GDTP Senior Level
Manufacturing Engineering Tech
SSG, U.S. Army
Taji, Iraq OIF II

 

[drawoh]

Iceman13,

Rephrasing the criticism here...

The GD&T goes on the feature, not on the construction lines. You cannot apply geometry and datums to pitch circles any more than you can apply them to centre lines. The positional tolerances go on the slots.

With positional tolerances on the slots where they belong, you can make an inspection fixture, but it will be a challenge. Your locating feature is less accurate than the slots. If you can add a clocking feature and get your drafter to re-specify datum[ ]B as three datum targets, you can centre the thing with a three[ ]jaw chuck.

Correction: Everybody can centre the thing with a three[ ]jaw chuck.

--
JHG

 

[Iceman13]

According to my customer contact the position of the slot pattern is described by the theoretical bolt circle of center points of those 36 slots.

The geometry of each individual slot however is not on center of a point placed .758" from the center point of Datum -B-. You will notice the bilateral tolerance zone for both the width and length of the feature. In past discussions I had been informed that the geometry segments are not drawn to the nominal values (low limit of size to use the customer's words) but instead have been created as follows...

1. Copy a point +Y distanced .758" from an origin point.
2. Draw a vertical line through the copied point.
3. Move that vertical line -X .043".
4. Copy a second vertical line +.084".
5. Draw a horizontal line through the copied point.
6. Repeat steps 3 & 4 in an identical manner respective to the horizontal line as size is dimensioned.
7. Trim excess tail to create the slot rectangle.
8. Rotate the rectangle 16° CW to the copied point.
9. Copy the slot and point 35 times CCW around the origin point at 10° CCW.

My subsequent issue then becomes that if a CMM is used to then check "true position" of the resultant bolt circle of the slot pattern, the measured point at the center of these slots as drawn has shifted by a shade more than -X: .0008" and +Y: .0008".

And anyone following or having replied in this thread will probably not be surprised to hear that my contact at the customer is adamant that GD & T as called out IS sufficiently correct for this drawing. Someone I am suspecting is not an engineer but once portrayed one in his junior high fall drama presentation.

Thanks for the replies thus far... good to know I am not coming completely out of left field on this.

 

[powerhound]

As we've all already said, this callout is bad. What they meant for the spec to say is completely different from what the spec is actually saying. A CMM will in fact check the true position of the bolt circle but how does that functionally matter? It doesn't. You can have half the slots stacked in one direction but at the correct radius and the other half of the slots stacked the other way. You can still have a perfectly centered diameter with the actual slot positions completely unusable.

The GD&T is bad...guaranteed.

John Acosta, GDTP Senior Level
Manufacturing Engineering Tech
SSG, U.S. Army
Taji, Iraq OIF II

 

[dgallup]

One of the fundamental requirements for a valid position callout is that basic dimensions MUST BE USED to establish the true position of the feature relative to the datums referenced. Do you see ANY basic dimensions on this drawing? I do not. Therefore, the position callout is invalid and thus you can not inspect it. There are many other problems as pointed out by others but it is just ridiculous to say the GD&T is correct.

----------------------------------------

The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.

 

[3DDave]

The basic dimension for the bolt circle is zero, as it is aligned with datum B and A. The problem is the slots appear to have no location tolerance and the circle has nothing to do with the slots. More specifically, there is no tolerance for the positions of the slots relative to the phantom circle or vice versa.

The centering problem is no problem - at least to the extent that it's exactly the same problem found when dealing with RFS diameters. Set the item on a precision turntable and use a dial indicator to check for the presence of at least two diametrically opposed or a set of at least three points that have the minimum radius relative to the turntable. It will take a while to nudge into position, but it can be done.

Once that is done, check for the location of the phantom circle. I'm sure it's exactly where it should be. The slots? Not a chance. Angle is dimensioned to air, and not to each other, so there's no location or orientation control among the slots.

Nice half-baked drawing. Too bad you're on the receiving end.