Eng-Tips is the largest engineering community on the Internet

Intelligent Work Forums for Engineering Professionals

Register Log in
  • Congratulations waross on being selected by the Tek-Tips community for having the most helpful posts in the forums last week. Way to Go!

Flatness in the absence of a GD&T callout.

Status
Not open for further replies.
tcogswell

tcogswell

Mechanical
Apr 6, 2011
6
0
0
US
I apologize if this has been answered in the past. I did see a post on concentricity but not flatness.

I have a part that has a thickness with tolerance called out but no specific flatness called on on it. The part does have a bow in it but the thickness is good through out. Is there an implied flatness in ANSI due the tolerance called out?
 
Replies continue below

Recommended for you

Sort by date Sort by votes
Assuming Rule#1 is a default condition (which should be the case if it is ANSI/ASME standard), flatness for each side of a feature can be as big as a tolerance value for its thickness.

Situation can immediately change if indepedency rule is invoked.
 
Upvote 0 Downvote
Yes as I understand it (assuming you mean ASME Y14.5), look up envelope principal if I recall the terminology correctly.

Essentially the entire feature has to fall between the stated dimensional tolerance for it's entire length.

Say you have a plate .500" thick +-.010" then including 'bow', the part has to fit in between parallel planes .510 apart. So you 'sort of' get a flatness of .020.

I can't remember the impact of 'perfect form not required at LMC but I'm sure one of the expert will chime in quick enough.

Posting guidelines faq731-376 (probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​
 
Upvote 0 Downvote
Is this drawing reflecting ASME Y14.5-94 (even 82) standard? Look in the notes section. If it does not, then there is no flatness requirement and the part could have a tremendous wow in it but still meeting specification.

If the drawing does reflect the ASME Y14.5 standard (I have a feeling it doesn't) and using Kenat's .500 +/- .010 example, we could have a flatness of up to .020.

Here is how to calculate the flatness. Measure the thickness of the part. Let's say it was .497. From the maximum part thickness of .510, subtract the actual thickness. In our case we would get .013 and that is the flatness allowed at that thickness. If the part was made at its largest allowable size, .510, there would be not flatness allowance.

Hope this helps.

Dave D.
 
Upvote 0 Downvote
tcogswell,

Let ma add some clarification (or maybe confuse you more).

If ANSI/ASME Y14.5 is invoked (or implied), you will have a "russian nesting doll" of tolerances.

I made picture (I like pictures) to illustrate it.

If you already read something about Rule 1, you know that your size tolerance is the largest one.
You can refine it with Parallelism. Your Parallelism tolerance zone will be "floating" inside of yours Size tolerance zone.
Then you can refine Parallelism with Flatness. Your Flatness tolerance zone will be "floating" inside of your Parallelism tolerance zone.

But there is a bright side to it. Because your Flatness is always smaller then Parallelism, you can measure Parallelism (sometimes it's easier) to make sure your flatness is good enough.

I am sure there are folks here who will be happy to discuss the issue further, so I am going back to work. :)

Link:

 
 http://files.engineering.com/getfile.aspx?folder=e2d14587-bf33-484c-ac71-fd99ff92ad94&file=FLATNESS.bmp
Upvote 0 Downvote
It is actually a piece of sheetmetal that is .125 thick and is called out as such. After the stamping out of the holes there is a bow in the part and no callout for flatness on the drawing. I am trying to figure out if it needs to go through a straightening operation to fall within the spec. and ANSI Y 14.5M 1982 is called out.
 
Upvote 0 Downvote
Does the bow make the part bad? Is the part not functional with this bow? To put a flatness on sheet metal part will be hard to control because of the stock sheet metal gauge size tolerances are relatively nice and tight. Unless you need the part to have a flatness that is better than the sheet metal gauge tolerance. To control the bow try using straightness applied to your sheet metal gauge thickness feature of size. This dimension will control your bow and get past the rule #1 perfect form at MMC.
 
Upvote 0 Downvote
SDETERS - I agree that a flatness requirement should be placed on the part drawing rather than relying on Rule #1. Rule #1 isn't well understood or utilized anyway.

Straightness is a component of flatness on allows a maximum bow in one direction only. I would still stick with flatness since if covers the complete plane.

Dave D.
 
Upvote 0 Downvote
I agree there should be a flatness called out, but there wasn't. I would like to know whether in the absence of said callout is there an implied one. If you measure the feature, in this case the thickness, it falls within the dimension and tolerance. The parts are being rejected for the bow and I am trying to figure out if there is a case to argue that they still meet spec.
 
Upvote 0 Downvote

Unfortunately, it looks like you have no case.

If ANSI Y 14.5M is explicitly mentioned and there is no note like "PERFECT FORM IS NOT REQUIRED AT MMC" or some other way to slip Independence principle in, things are exactly like on my picture: tolerance you are given should cover EVERYTHING including the bow.

Good luck!
 
Upvote 0 Downvote
tcogswell, I had a very similar situation recently but from the other side. A vendor sent us parts that looked like giant pringles potato chips.

Our QA guy was going on about how we don't have a flatness so couldnt' reject them.

I pointed out the rule 1 and I think we forced the vendor to replace the parts.

Posting guidelines faq731-376 (probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​
 
Upvote 0 Downvote
I would be careful... if it is sheet metal, then we potentially have a non-rigid part. And non-rigid parts are exempt from ASME's Rule #1, thus making it equal to the PERFECT FORM AT MMC NOT REQD note, without having that note on the drawing.
So there are two questions: Is the drawing referencing an ANSI/ASME standard? And should it be considered as non-rigid? (i.e., will it normally bow in its intended function?)

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
 
Upvote 0 Downvote
Belanger,

The drawing calls out ANSI Y14.5M 1982. It is a cover that gets screwed down on all four sides. One would think even with a bow it would flatten being screwed down and all, but they did not stipulate a contrained condition.
 
Upvote 0 Downvote
John-Paul,
I think to declare a part non-rigid, the drawing must have a note stating that "All tolerances apply with datum feature(s) x restrained". Without a note similar to this, the default of measurement in the free state applies and the part is considered rigid.

I agree that you're still correct regarding rule 1 though, since sheet metal parts are "from stock", so 2.7.1.3 of Y14.5M-1994 applies. So even if Y14.5 is referenced on the drawing, I think a sheet metal part needs an explicit flatness spec if that is the functional requirement.

Dean
 
Upvote 0 Downvote
That brings up a good question, Dean. I don't have a copy of the standard in front of me today, but I don't think we can say that the default condition being free state equates to a proclamation of having a rigid part. But maybe it's one of those things that is open to interpretation. (Heck, anything is non-rigid if you put enough force on it!) Thoughts?

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
 
Upvote 0 Downvote
Hi Jean-Paul,
Yes, I agree that a "floppy" part being considered rigid just because it's not restrained for measurement is odd... I'll run through my thoughts on this & I'm sure you or someone else will straighten me out if I'm off track... I'm relatively flexible about this topic.

If a part is considered flexible relative to the mating assembly, then it should be restrained for measurement, since restraint to an ideal mating assembly (a fixture) is likely the best way to model the part's functional state.

If the part is not restrained for measurement, then the assumption would be that restraint was considered and not selected, so the part is probably relatively stiff compared to the mating assembly, so the free state best models the part's functional state.

So, if a non-rigid part is dealt with by restraining specific datum feature(s) to a fixture (probably only one datum feature, since restraint to more than one often causes repeatability problems) then I would say that it follows that a part is considered rigid, per Y14.5's use of these words, if it is not restrained for measurement. I'm using figure 6-54 in Y14.5M-1994 as my justification for saying this (a student accidentally put my Y14.5-2009 in their backpack last class & I won't get it back until tomorrow, so sorry for a '94 only reference).

Dean


Do you agree?

Dean
 
Upvote 0 Downvote
Well, I'm away for a few days, so I don't have either version of the standard in front of me :)

But I still hesitate to agree that a non-restrained part is automatically assumed to be rigid.

How would we dimension/tolerance a length of garden hose? Must I put a note on there telling everyone how to restrain it?

This topic also brings up the circled F modifier, but I see that as only a way to temporarily override a general restraint note. I don't see it as declaration of non-rigidity. Maybe I should have started another thread on this aspect...sorry!

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
 
Upvote 0 Downvote
Status
Not open for further replies.

Similar threads

ericscottf
  • Question
Proper GD&T for interrupted threads?
Replies
14
Views
95
ericscottf
ericscottf
looslib
  • Locked
  • Question
Position of CD&T callout
Replies
4
Views
23
3DDave
3DDave
efulm4444
  • Locked
  • Question
GD&T Question - Properly Defining a Global Tolerance
Replies
2
Views
23
drawoh
drawoh
Martin_K
  • Locked
  • Question
GD&T Flatness question
Replies
15
Views
49
Martin_K
Martin_K
DimaM
  • Question
GD&T: How to inspect tertiary datum feature position tolerances?
Replies
7
Views
42
Burunduk
Burunduk
Back
Top