Straightness tolerance on a piece of sheetmetal 1

[BraunP]

Hello everyone,

I am still leaning GT&D. Can you look at my print for the straightness tolerance. I need this piece to be straight. As of right now I have the tolerance set on both sides of the piece, but I have a feeling I cant put a tolerance on a datum. Help please. Thank you for your help.

 

[KENAT]

First off, are you sure straightness is the control you want?

Or do you really want the 'A' surface to be flat and the other side to be parallel to it within some reasonable limit?

You can apply a control to a surface you then derive a datum from.

Posting guidelines faq731-376

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

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

 

[JNieman]

(assuming inches)
.075 thick, 3.32x6"... measure it in the restrained state - easy fix

Anyways - I'm betting you were intended to apply flatness.

Criticism:
Applying flatness of .005 to both sides it going to impact the costs of the parts - most people are going to either fail to meet the tolerance, or they're going to want to buy extra thick stock material and grind both sides, jacking up the cost of these parts tremendously. I think you should really examine what you -NEED- from the thickness, flatness, and parallelism of that part. Especially considering that it's .075 thk and likely not going to be all that rigid. You said no more than "sheet metal" so I'm assuming 14ga cold roll mild steel.

It's one thing for the GD&T (not GT&D) to be 'valid' callouts, but another thing for them to be appropriate callouts. The GD&T must match the design requirements, or you're just imparting undue cost and possibly getting a lot of "no bid" responses to the RFQs, or getting a lot of cussing from the manufacturers and QA folk.

Anyways... long story short - look into flatness and parallelism controls.

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

 

[BraunP]

1) GT&D, looks like I had a dyslexic moment.
2) i was actually trying to figure out what would be better, straightness or parallel. For my application, a flatness would not work because it is a part that is in between 2 feed screws. and if I understand flatness correctly, that surface needs to be within 2 parallel plans around the theoretical surface. meaning this though have a "angle" to it.

The reason I used straightness is because this part needs to be, well straight. I did have a prototype made up and it came in bent, which interfered with the screws and caused wear and resistance. My worry with parallel is that the entire thing can be parallel but at an angle.

Trust me, I would not be using GD&T is I did not need to. Because that prototype part came in with a noticeable bend, I am trying to eliminate that problem.

I think I should have added all this detail to begin with. The bend happened at the .881 hole. form corner to corner.

Now that I think about it. parallel probably would work the best and have it reference to datum A

 

[DiegoLGraves]

FWIW, if this is a steel or aluminum material, as a fabricator I'd quote a laser-cut part if you specified flatness on one surface and stock material tolerance on the thickness. Per the linked sketch I'd no-quote it, and certainly wouldn't consider punching the part. Punching tonnage in mild steel would be about 4 tons plus stripping force, and would likely bend the piece outside of tolerance, even if it came in flat from the vendor.

Diego

 

[3DDave]

As a side-note - one should not apply a material condition modifier to a surface callout. There should be no (M) assign to straightness of a surface. You might use (M) if the straightness was applied to the thickness of the material, though flatness is applicable in the '2009 version.

Also, GT&D is really more correct. There are Geometric Tolerances, but no Geometric Dimensions, at least not defined in any spec.

 

[BraunP]

FWIW, if this is a steel or aluminum material, as a fabricator I'd quote a laser-cut part if you specified flatness on one surface and stock material tolerance on the thickness. Per the linked sketch I'd no-quote it, and certainly wouldn't consider punching the part

My company has been having some problems with our current sheet metal vender. when the piece came in, it was out of the old tolerance. luckily for the vender, since this was a prototype just to prove that, yes we can make the assembly, and yes it works (prove to management) we let it slide. But for production quality it is unacceptable.

I dont want to use flatness because I need the part "perfectly" straight. and flatness, if I understand correctly just pertains to that one side as oppose to the part as a whole. It seems the best option for what I need is parallel.

 

[KENAT]

BraunP, unless I'm missing something I believe your understanding of flatness may be wrong.

Flatness says a specific surface is 'flat' to within some limit.

Parallelism says a specific surface is parallell to another surface within some limit.

So, often one does something like make bottom surface 'flat' and top surface 'parallel' to the bottom surface.

Posting guidelines faq731-376

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

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

 

[BraunP]

ok, I was incorrect on my understanding. GD&T is a little confusing. From what I have gathered, doing the flat with parallel will meet my needs. This pressure is too much =P

 

[ewh]

GD&T is still correct... the standard does define general dimensioning rules, and most parts do happen to be geometric. ;-)

"Know the rules well, so you can break them effectively."
-Dalai Lama XIV

 

[3DDave]

And yet so many references to Geometric Dimensioning and Tolerancing, as per these guys

https://www.asme.org/shop/certifica...-y14-5-geometric-dimensioning-and-tolerancing

who should have just used the title of the spec they are certifying people for. Not that hard.

The title of the spec is just Dimensioning and Tolerancing; no "G" word.

In an early work it was "Geometric and Positional Dimensioning and Tolerancing," which predated ASA Y14.5-1965, by Lowell Foster. This leaves questions within the area of Y14.5:
1) What is a geometric dimension?
2) What is a positional dimension?
3) What is a dimension that is neither geometric or positional?
4) If basic dimensions are used as coordinates to locate a feature are they coordinate dimensions? If not, why not?

Frankly I'm blaming Lowell for popularizing the undefined terminology.

I figure if the 1982 and 1994 editions could not define a 'geometric dimension' and the 2009 version doesn't mention it in the body, then it's time to give it up. Using the more accurate phrase "put some FCFs on the drawing" more accurately describes what people imply when they say "put some GD&T on the drawing." Lowell doesn't define any of it in his early work, and it's not likely defined in any later one.

 

[Ganeshphapale]

As per your drawing i will suggest that dont give tolerance to the datum.
as per engineering std datum should be true.

 

[3DDave]

No tolerance can be applied to a datum on a drawing because a datum is an idealized geometry that is perfect.

One can apply a tolerance to a datum simulator in the jig or fixture or as part of a CMM analysis software. One can apply a tolerance to a datum feature, which does appear on the drawing and should be done to limit the uncertainty in comparing the datum feature to the datum simulator.

 

[CheckerHater]

GD&T is a little confusing... This pressure is too much =P

BraunP,

I understand your struggle. If you are trying to achieve deeper understanding of GD&T (or should I say GPS), try to get your hands on this book:

http://www.iso.org/iso/home/store/publication_item.htm?pid=PUB100296

It may be lacking finer details of practical applications, but has very good explanation of underlying concepts. (I am assuming you are coming from BS ISO world)

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

 

[KENAT]

Pretty sure the OP is US based CH.

Ganeshphapale I'm afraid you are mistaken, it is often appropriate to place a control on the datum surface/feature from which the datum gets derived.

Posting guidelines faq731-376

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

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

 

[CheckerHater]

I know, I know. I submitted thread for deletion but administration is not in the hurry :-(

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

 

[BraunP]

I am going to have to read up on a lot of this stuff. And yes KENAT I am US. ok, just thinking, if I just specify a parallel on one side and nothing on the datum side. theoretically the part can have a .5" bend, and if it is parallel with the datum within the tolerance, it is acceptable. so to keep the datum flat or straight ( I am leaning towards straight as oppose to flat) that will keep the piece vertical, and the parallel tolerance will hold the other side correctly. Does that make sense?

 

[Belanger]

I figure if the 1982 and 1994 editions could not define a 'geometric dimension' and the 2009 version doesn't mention it in the body, then it's time to give it up.

I think a mountain is being made out of a molehill. Indeed there is no such thing as a "geometric dimension" because those two words were never meant to stand alone together. Instead, "geometric" is an adjective defining a whole philosophy of "dimensioning and tolerancing" taking those words as a complete unit. It that sense it is quite different from the traditional -- and myopic -- philosophy of dimensioning and tolerancing. It needn't focus solely on the fourteen symbols.

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

 

[KENAT]

BraunP - no.

Assuming you are working to ASME Y14.5 (and this is referenced by the drawing or purchasing contract) then the tolerance on material thickness also has a second order control on flatness due to 'rule 1/Taylor principal' - unless you deliberately override this.

Your drawing extract doesn't show what the tolerance is on the .075 dimension, lets assume it's +-.005. In this case if the material was .07 thick you could have up to .010 deviation from flat.

Pretty sue you want flatness not straightness straightness only applies in one direction while flatness is planar.

Posting guidelines faq731-376

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

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

 

[pmarc]

And yet so many references to Geometric Dimensioning and Tolerancing...

Dave, you will not give up easily on the "GD&T vs. D&T" thing, will you?

I agree with J-P, it is minor issue. As long as rules defined in the Y14.5 or any other standard are followed correctly, one can call the entire thing D&T, GD&T, GT&D, GPS or even NHL or NBA. This will not make any difference to drawing interpretation and, what is even more important, to functional requirements of the design.

The real problem - and here we should indeed focus on using correct terminology - is when somebody, for example, is saying that a datum feature should not be controlled for its form because it is a datum, and as such is perfect. This creates real issues. No wonder there are so many drawings out there that show datum features totally uncontrolled for their form and mutual orientation/location.

No wonder there are so many folks that keep applying concentricity tolerance on ASME prints while what they really mean/need is coaxiality (position) tolerance.

These are areas where using proper terminology makes the difference. This is where real money can be saved.

Just my 0.02$.