How to establish the Datum-C ?

[Madhu454]

Hi All,
I am designing a flange, which is used on the wind turbine blade root for mounting the blade to Hub. Flange thickness is 30mm. I am facing some difficulties in assiging the GD&T.Please see the attached drawing.

Function of the part:
The datum feature A which mates with the plane established by number of bushings on the blade root.
The holes 33 +0.5/-0 is the clearance hole for the bushings (equally spaced on BCD). Hence by considering the function, the pattern of holes has been considered as the datum feature B. Now the datum B will be the axis (formed by intersection of two perpendicular planes passing through datum axis B). datum-B can be established using a fixed guage pins (32.6mm) located at true positions.

We also have some tapped holes (M10x1.5-6H) which is drilled on the cylindrical face of the inner diameter of the flange. shown in red font in the attached drawing. To position these holes can I use additional datum-C, inorder to lock the rotational oriention of these holes?

1)Now the problem is if I use any one of the hole as a datum feature-C, then how do I establish the datum-C? because to establish datum-B, we use fixed guage pins which is already present inside of the hole which is identified as datum feature-C.
2)How the position of the tapped holes is affected if I remove the M modifier from the FCF which is associated with datum-B.
3)How the position of the taped holes is affected if I give M modifier to the Datum-C

Hope you understood my question. Can any one help me in better way of dimensioning this?

 

[Belanger]

Can't access the file -- is there an extension? (jpg, pdf, etc.)

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

http://www.gdtseminars.com

 

[CheckerHater]

For the beginning, don't use symbol "&" in the file name.

 

[Madhu454]

Hi,
Now the drawing has been attached. Please let me know your opinion.

 

[PaulJackson]

The pattern constrains the remaining three degrees of freedom not constrained by [A] so adding [C] to the control is irrelevant if not erroneous.
Paul

 

[CheckerHater]

I agree with Paul Jackson here.
Datum C will not do anything more than datum B already did.
On second question, shortly, you will eliminate “datum shift”, but you may end up with more complicated/expensive gauge setup.
Since datum C seems to be irrelevant, third question may probably be left without answer.

 

[dingy2]

I would agree with Paul and CheckerHater that a tertiary datum is not needed. Datum B is sufficient for locating the tapped holes on the inside of the flange.

There is something that could be improved on the drawing. Having positional in RFS while the datum feature of size is in MMB doesn't make sense to me although it is legal. Love to see the gage for that one. I would suggest either having positional in RFS and datum in RMB or positional in MMC and datum in MMB (preferable for gauging). Just a thought.

Dave D.

http://www.qmsi.ca

 

[pmarc]

I would be rather worried about lack of reference to primary datum A in those positional callouts to B(M). Inspection repeatability may be really poor, not mentioning that having so many different datum reference frames on such part looks at least suspect.

Another thing - right now I do not see a basic dimension from datum A to tapped holes centers defining true position of tolerance zones properly. If this has not been shown just because it was not the clue of your questions, please ignore it. But if it is missing in reality, make sure it is there.

As for soundness of "having positional in RFS while the datum feature of size is in MMB", we had a discussion not so long ago in this thread:

http://www.eng-tips.com/viewthread.cfm?qid=329956,

but unfortunately I did not get any answer to my question.

P.S.: I am with those saying that tertiary datum feature is not needed for correct positioning tapped holes.

 

[Madhu454]

Hi All,
Thanks for your inputs. I have created the drawing as per ISO std. Attached the new drawing.
Please see if it looks okay?

Also I would like to know below concepts
1) In the drawing I have called out parallelism callout. Can the parallelism be called out on unit basis, like how I called out on flatness?
3) Also I don’t know how the M modifier for the tapped holes will help? I was suggested to use RFS condition for threaded holes while using position control. Hence I have not included M modifier for tapped holes. Can anyone help me in understanding this?
2) I don’t know how CMM machine works and how to do the measurement. At present to design a gauge and manufacture it will take long time. We want this flange to be measured in CMM. Just curious to know how this part is measured in CMM.
a) How do they establish the datum-B in CMM?
b) How do they consider the datum shift concept?

 

[bxbzq]

Are you sure you are going to build gage to simulate datums and inspect positions for such a relatively big size and low volume part?

 

[fsincox]

I am glad to see this, I understand people have trouble with the concept of a pattern of 20 some holes being a single datum and, is it, or, is it not, accepted. My understanding of the concepts and the "bible" says, finally, it is. I remember when I got in trouble for unsing a pattern of 2 dowel holes as a secondary datum. (wink, they only want edges as datums, pretty hard on a part like this).

 

[aldumoul]

It is my understanding (corect me if I'm wrong). That you cannot get bonus tolerance on B for the tapped holes? Because you are establishing 2 planes for datum B. So, is the B(M) in the FCFs inapplicable?

 

[Belanger]

No, aldumoul, it's OK to have that. In fact, from a practical point of view we must have "M" after datum reference B, because it is a group of features. That extra looseness doesn't get added directly into the position tolerance of the tapped holes, but it does allow the tolerance zones for all those tapped holes to shift. (That's why it's usually better to say "shift tolerance" rather than "bonus tolerance," which is more properly reserved for the "M" when it's shown directly after the tolerance number.)

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

http://www.gdtseminars.com

 

[aldumoul]

Got it