Flatness call out for partial surface 1

[Cyeazel]

Hello

I was wondering if anybody had some advice on the proper way to call out a flatness tolerance using GD&T but only for a partial surface. The application is a mechanical seal. I've attached a drawing for illustration. The surface in question is labeled datum A with the .001 flatness call out. The only section of the surface that requires this control is enclosed in the rectangle. I'm just not sure how to properly notate this call out on the drawing. Thanks in advance for any advice.

 

[JNieman]

I would call out two points, a start and end, defining the extent of the controlled area, and use a FCF with a "between" symbol. The 'between symbol' is described in 3.3.11 of ASME Y14.5-2009, for example.

_________________________________________
NX8.0, Solidworks 2014, AutoCAD, Enovia V5

 

[Belanger]

Do you want the datum to also be taken as the local area, or should datum feature A remain as the full surface? (The answer will impact the suggested answers.)

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

 

[Cyeazel]

Thank you for your response. That is helpful. I appreciate it.

 

[KENAT]

I've done variations on what JNieman says.

If you're using the surface/portion of the surface as datum that does add another level of complexity as Belanger mentions.

I've also introduced functionally unnecessary steps on a surface to help clarify which area needs tighter control but that's a last resort to me - though in some cases may help with likely manufacturing methods.

Posting guidelines faq731-376

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

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

 

[CheckerHater]

Chain line.

"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future

 

[Cyeazel]

Thank you all again for chiming in. I've attached another image of the drawing with the changes based on the suggestions here.


I noticed your response after I updated the drawing. In what way will this impact the call out?

 

[SDETERS]

Could this fall under the limited length callout? 1.7.3 ASME Y14.5 2009 standard?

 

[Belanger]

I asked about the datum because the datum feature symbol is attached to your flatness callout. So it could be interpreted that whatever "limited length" you want to impose on the flatness also gets imposed on the datum feature. Thus my question.

Given your latest picture, I would probably go with the chain line suggestion rather than the "between X & Y" arrow.
Also note that the flatness tolerance would still be seen as extending into the picture for the full surface depth, within that strip of .247. If you wanted a limitation in the depth direction also, then you'd have to do something else to indicate that.

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

 

[CheckerHater]

Could this fall under the limited length callout? 1.7.3 ASME Y14.5 2009 standard?

Yes, indeed.

Also, the purists may note that use of reference letters was defined for Profile tolerance and they are expected to indicate "extremities" of the features, that is, places where the features end rather than arbitrary points in the middle of said features.

"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future

 

[dgallup]

While I think that is a valid flatness specification I think your manufacturing engineer will throw it back in your face. This is obviously a revolved part from the diameter dimensions and run out specifications. You are carrying the flatness all the way into the inside corner at point X. You need to either allow some corner radius or an undercut, there is not such thing as a perfectly sharp inside corner.

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

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.

 

[Cyeazel]

I've made some adjustments. I used the chain line instead along with a reference diameter to indicate where the flatness spec is needed. I also included the radius dimension for the inner corner which I had previously forgotten (Thank you dgallup for the reminder).

I asked about the datum because the datum feature symbol is attached to your flatness call out. So it could be interpreted that whatever "limited length" you want to impose on the flatness also gets imposed on the datum feature. Thus my question.

Yes, the datum feature will only be the the area of the surface indicated by the flatness call out and chain line. I've attached another updated drawing.

 

[Belanger]

Regarding the flatness and datum thing for the local area, I think it's pretty much OK now. On an unrelated note, maybe add a "CF" (for continuous feature) or similar notation on the 3.352 diameter so that it's clear that the diameter and the total runout tolerance are for the entire feature on both sides of the cutout. Otherwise that cutout/slot makes the requirements stop as soon as you get to the cutout/slot.

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

 

[Cyeazel]

Ah yes, I will add that too. Thanks for pointing that out. Thanks again for the advice. I very much appreciate it.