Interpretation of datum -C- 1

[DoogieP]

Greetings All,
My customer is rejecting this part claiming that the lower pattern of M3 holes are out of tolerance. When I check them the worst TP I get is about .028mm they are getting TP around .380mm. When I setup and measure I'm implying the bottom surface is parallel to datum A-B not shown in this view but, is an axis of 2 concentric diameters from which all the basic dimensions to said holes originate from. I also imply that Datum C is perpendicular to this surface since it's the surface from which I fixture from. I can then zero out on the large center hole and measure the 25,42, 55 and 60mm basic dims. Then I rotate the part 90 degrees making sure A-B is parallel to my surface plate, zero off the bore and proceed to check the hole that falls on datum -C-, 2, 28 and 30.5 mm dimensions. The are aligning datum -C- off the 2 small surfaces of the 30 degree notches which based on the angular tolerance can vary far more than the locational tolerance of the hole pattern so, I would consider this unusable as a datum feature for this reason. When I had the part setup at 90 degrees (rotated cw to view in drawing) I checked the location of these surfaces and the surface that would be to the right of the bore measures about +.1mm and the surface to the left measures around -.1mm which would skew this pattern. Am I correct in how I'm setting up to measure? Let me know if you need more info. Thanks for any feed back.

Doug

 

[greenimi]

Cannot open the file. Does not have any extension, maybe that's why....

 

[DoogieP]

It didn't like something about the original name so, I shortened it up to just 3 letters. A thousand apologies oh exalted one. I was able to open it through the link

Doug

 

[3DDave]

The original filename has an "&" in it.

It would be easier to understand if it included the original callouts for the datum references. A datum should never be applied to a centerline.

It also leaves me unsettled to 'imply' a datum reference. It's either explicit or it doesn't count.

 

[KENAT]

Hmm, datum C is a bit ambiguous unless I'm missing something.

Being placed on the Centerline extension I'd guess it's meant to be a plan on the axis of one of the diameters - I think the A-B you mention supports this.

However, it's not entirely clear what the 'clocking' feature is.

Could be the small hole at the bottom though that looks just off the center-line.

I don't think it would be the 30° notches as you can't tell which it is and being both conflicts with it being a plane on the axis.

What does the customer claim datum C is?

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[greenimi]

Couple of questions:
1.What is the datum compound A-B?
2.Datum feature C shall not be placed on the centerline, but on an actual feature. So, datum C is the axis of what feature?
3. Same question as above for datum feature D

Just make sure you abide to the rule of higher precedence datums. A-B probably will arrest 3 or 4 degrees of freedom. (3 if they are planes and 4 if they are axes). Then C will arrest the remaining ones--if capable. Then, finally D the ones left DF (s) if impose by the functionality of the product.

 

[DoogieP]

3DDave, I had nothing to do with the design. This component was designed by one of my customers. They are through all of their FDA testing and are approved to start production. They are an R&D house so, they contracted another company to start manufacturing. The designer of this part is more fit, form and function driven and most of their prints are severely over tolerance. Their manufacturing engineers are fully aware of this and are trying to go through and tidy up drawings as quickly as they can. The downside is that he contract manufacturer is being reluctant to go back to the designer and we have asked the designer for guidance and their response is "you need to work through the other guys on this". So I'm between a rock and a hard place. I'm just trying to get an interpretation on establishing a frame of reference.

 

[DoogieP]

KENAT, it is ambiguous and one of the small holes is on that centerline which, if you use this feature to clock datum C then everything falls into place. If you use one of the edges of the 30 degree openings then everything is skewed.

the customer is using the edge of one of the 30 degree opening and I agree with you on its usefulness as a datum feature.

 

[DoogieP]

greenimi,
1. A-B is an axis through 2 concentric bores which is at the intersection of datum C and the horizontal centerline of the large bore
2. I interpret datum C to exist on the axis of A-B that passes through one of the M3 holes
3. Datum D exists on a face on the opposite side of the view I supplied that is perpendicular to A-B

 

[DoogieP]

Here is the view showing A, B and D

 

[3DDave]

With no definite datum C, you are stuck. Per your last diagram, A-B is redundant with D in the hole callouts. Had the order been [D|A-B] then it would work to have A-B refine location, but A-B as primary nails the orientation and D cannot affect it. Maybe it is there for establishing a simultaneous relationship with other features.

You should have determined what they thought was the clocking feature before machining the part instead of guessing. Live and learn. Nothing on the drawings so far clarify the orientation or location of datum C.

 

[TheTick]

I've rejected customers' drawings like this before. Won't touch them unless they either fix them or stipulate in the contract that the drawing is ambiguous.

 

[DoogieP]

Thanks for all the feedback, I have a conference call at 9 and will suggest to my customer that datum C is ambiguous and we need clarification on which feature is datum C

 

[mkcski]

I agree with TheTick. Be VERY cautious when quoting to drawings with misapplied GDT - especially datums and their sequence in in the FCF's. I am in estimating, and with a drawing like yours, I would define in writing with marked up drawings, my interpretation the ambiguous requirements and how the part will be inspected to confirm requirements. This opens the door for negotiation and avoids future misunderstandings.

One problem with this approach is you assume the person on the other end understands GDT. But given the "bad" drawing, they most likely do not. So a learning session on their part may be necessary to get your response understood. Telling the customer they don't know GDT is dangerous. Tread lightly. Of note: this is one reason why I participate in this forum; my responses help with my written GDT communication skills

Certified Sr. GD&T Professional

 

[powerhound]

Just to echo everyone else here: this print is ambiguous at best. In case they ask Para. 4.8.2 in ASME Y14.5-2009 is where it is stated that datum feature symbols are not to be placed on centerlines.

John Acosta, GDTP Senior Level
Manufacturing Engineering Tech

 

[DoogieP]

Customer agreed to make one of the M3 holes the clocking feature, all is well. Thanks for the feedback

 

[TheTick]

It's wonderful what can be negotiated when you start talking.