Design intent versus proposed drawing update. 1

[greenimi]

I have a quick question for the GD&T experts. Should be an easy one for your level of expertise.

See drawing attached:

- Picture A is the original design intent
- Picture B is the proposed one (proposed one is to make this part inspected by a functional gauge, a simple go functional gauge, NOT an assembly with multiple pins, etc)

Question: By changing the positional callout from Ø.005 to Ø .002 are we keeping the design intent? decrease with Ø.003 (Ø.003 is from the additional datum shift allowed by adding M at the Datum Reference Frame: .378-.375 =.003).

What is your opinion about this approach? Will hold some water?

Note: Engineering is okay to make the updated print more tight/stringent requirements, but NOT to relax any of these requirements.

I kind of know that this approach could be valid (if it's valid) only in this special case (only one feature to be controlled relative to a datum, and NOT valid with multiple features/ patterns).

Again, is this concept valid from your point of view? Any thoughts?

THANK YOU FOR YOUR HELP!!

 

[dingy2]

How does the part function? Is there are cylindrical feature that protrudes into the datum A hole? If the answer is "yes", then reference it at MMB and leave the tolerance at .005 in the feature control frame. Your drawing now simulates the function of the part.

The original drawing did not reflect its function when the datum hole was in RMB.



Dave D.

http://www.qmsi.ca

 

[greenimi]

Quote: "How does the part function? Is there are cylindrical feature that protrudes into the datum A hole? If the answer is "yes", then reference it at MMB and leave the tolerance at .005 in the feature control frame. Your drawing now simulates the function of the part.

The original drawing did not reflect its function when the datum hole was in RMB."

Engineering is not comfortable to allow any datum shift except what is allowed NOW on the original drawing. So we cannot just add MMB on the DRF without having to give up some tolerance.
As per their statement it's not the function of the part and that's why they have it RFS at the datum structure (DRF) in the first place. So we have to keep the design intent unaltered.

 

[pmarc]

What is exactly the desing intent? Is it to keep offset of both axes of holes unchanged regardless of dimensioning scheme, even if those schemes do not reflect the same function of the part in an assembly?

 

[powerhound]

I agree with Dave but we need to know more about what the OD is related to. Depending on how the OD is related, an MMB modifier can actually hurt the function of the part. Simply taking tolerance from the feature control frame and allowing an MMB modifier of the same amount does not equal the same thing.

Powerhound, GDTP T-0419
Engineering Technician
Inventor 2010
Mastercam X5
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[drawoh]

greenini,

Your drawing[ ]A allows a maximum positional tolerance of Ø.005". Your drawing[ ]B allows a maximum positional tolerance of Ø.005" at LMC. As you note, this allows the use of a gauge to test for positional error. The original specification was harder to inspect.

Anything conforming to drawing[ ]B meets the requirements of drawing[ ]A. Some items conforming to drawing[ ]A, and to the design intent, will be rejected as per drawing[ ]B. What your guys are doing is tightening the tolerances to simplify inspection.

This practice violates one of the objectives of GD&T, namely, to allow as many functional parts as possible. I am curious as to how much actually is saved by this aspect of GD&T. I would expect to save anything unless my manufacturing process is marginally able to achieve tolerances.

Would it be possible for you to keep drawing[ ]A, and let manufacturing organize their work any way they darn well please, i.e. as per drawing[ ]B? A lot companies maintain engineering drawings, and manufacturing drawings.

JHG

 

[greenimi]

pmarc quote:
"What is exactly the desing intent? Is it to keep offset of both axes of holes unchanged regardless of dimensioning scheme, even if those schemes do not reflect the same function of the part in an assembly? "

pmarc

Per what I was explained by the engineering that is an alignment concern, axes of two or more diameters must be aligned. A tolerance stackup analysis has been done for the assembly and has been concluded that the best GD&T scheme is the one depicted (drawing A)= best GD&T scheme means to allow as many functional parts as possible. Again, I was told that a pin must fit in the hole(press-fit). It must be assumed that the pin follows the hole.

 

[pmarc]

If there has to be press-fit assured (I assume between datum feature A hole and its counterpart pin) then I would say scenario B is at least suspect, because it does not reflect the design intent by nature.

It is true that both scenarios result in the same maximum offset of axes (.0075), but B scheme does not simply assure pin always following the hole, plus position tolerance in unnecessarily tightened.

If the alignment is a major concern, I think position at MMC is not a good choice too, because the alignment depends on the size of toleranced hole, means:
- hole at .510 -> greater possible misalignment;
- hole at .500 -> smaller possible misalignment.

 

[greenimi]

pmarc,

I agree with you that scenario B is kind of suspect, as has been made to help inspection qualify/inspect the positional requirement. As "drawoh" said, they want to sacrifice some manufacturing tolerances for inspection purpose.

That was also my feeling, that everything to pass drawing B will 100% pass drawing A, but I was not sure and that was the reason for the posting.

And yes, the position tolerance is unnecessarily tightened (scenario B), but I guess that's the price they have to pay for using a single piece functional gauge instead of a functional gauge with multiple pins (to simulate datum A RFS) or a CMM.

I guess you agree with "drawoh" posting above.
Thank you for your input.

 

[pmarc]

Yes, I basically agree with drawoh's post, though to be honest have no idea where the numbers for maximum positional tolerance stated in the first part of his post came from. Can someone enlighten me? I must have a blackout, or...?

 

[drawoh]

pmarc,

I ignored the MMC(B) specification on the 0.500 diameter, because it was on both versions. Actually, I should have added .010" tolerance to both maximum values.

The LMC condition of the datum provides .003" allowance, that I added to the positional tolerance of the other hole. .002"+.003"=.005".

JHG

 

[TheTick]

Follow the money; do the math

Original has a larger tolerance, thus likely cheaper, but gage and inspection cost more.

New version is faster and cheaper to inspect, but tighter tolerances.

Which is cheaper? Depends on cost and capabilities of the processes involved.