please help clarify a fundamental of GD&T 1

[hobbs101]

Hi. I've been using GD&T for a few years now. I was hoping someone could help me with one thing that I don't fully understand.

See attached simple part drawing. This is done in the dimensioning style that I know.

What I don't fully understand is that the circular hole is dimensioned using the GD&T dimensions, but the square cutout is dimensioned using traditional style coordinate dimensions.

If I wanted to tolerance the cutout in the same way as the hole then I'd have to apply GD&T tolerances to each of the surfaces wouldn't I? I guess this is because there is no common axis.

Is there anyway to control the position and size of the cutout using GD&T?

Anyway, am I correct in what I say? I'd appreciate others views on this point.

Thanks.

 

[pmarc]

Hobbs101,
There are different ways to control position of rectangular cutout by GD&T. You can for example...:
- apply two positional FCFs wrt |A|B|C| to width (25.0) and height (15.0) of the slot and locate center planes of the slot by two basic dimensions (22.5 & 67.5) originating at bottom left corner of the part, which is datum reference frame origin;
- define width/height/corner radii of the slot by basic dimensions, locate the true profile from DRF origin either by basic dimensions to slot's center planes or by basic dimensions to sides of the slot and apply profile of surface FCF wrt |A|B|C| with all around symbol;
- combine profile FCF with positional FCF as shown in fig. 8-24 of Y14.5-2009 (though I am not sure that this method will be clear for ISO prints users).

As a GD&T purist, I strongly recommend not to use traditional dimensioning to locate square holes (or any other type of features). It is not that it is illegal or even ambiguous. I just think that there are very few applications that require 2 out of 4 side walls of the cutout (in this case, bottom and left) to be related to datum feature surfaces (B and C here) and not to perfect DRF, independently of what happens with actual surfaces B & C.

 

[CheckerHater]

There are different ways to control your rectangular cut-out.
The enclosed sketch shows just the basic ideas.
The width of the cut-out is what is called “feature of size” (just like the round hole), so it can be controlled in similar manner.
If the entire outline with all of its features is equally important, then Profile control may be used.
You mention using GD&T for years, so you must be in possession of a book or two. Give them the closer look.
Good luck!

 

[KENAT]

I think CH and pmarc have you covered hobbs but just in case I throw 2C in.

No you don't have to apply GD&t to each surface individually, and in fact for a regular feature of size like your square cut out there is effectively an axis for the feature.

http://www.tec-ease.com/gdt-tips-view.php?q=129

Posting guidelines faq731-376

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

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

 

[hobbs101]

Thank you all for the replies. It's starting to become a little clearer. Yes, I learnt GD&T some time ago from the Alex Krulikowski book, but since then I think I've been given some bad advice from colleagues on the way things should be done and am now very confused!!

I'm looking through the book now just to brush up on a few things, but perhaps you can help me with another fundamental question ...

I've always considered that basic dimensions are ONLY used to control the position of a feature, e.g. a hole. The size of the hole itself is controlled by a tolerance such as Dia10 +/-0.1. But, is this not the case? Is it true that the hole itself could have a basic dimension of Dia10, with a FCF controlling it's surface profile?

Maybe to ask more simply
- in a drawing could ALL dimensions be basic dimensions, as long as all surfaces has FCFs controlling their positions?

Thanks again.

 

[Belanger]

Yes to both questions (if we change your last word from position to profile).

Basic dimensions are used to establish the "true profile" which a profile tolerance will then control. So if a profile tolerance is applied to a hole, the diameter MUST be a basic dimension.

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

http://www.gdtseminars.com

 

[CheckerHater]

- in a drawing could ALL dimensions be basic dimensions, as long as all surfaces has FCFs controlling their positions?

Yes. And sometimes you may not even need dimensions, but declare the entire 3D CAD model "basic"

 

[hobbs101]

Ok, it's becoming much clearer now!

Belanger, you say changing my last word to profile rather than position, but surely the surfaces can be controlled by positional tolerance also?

It seems to me that within GD&T there are different ways of dimensioning, all of which are correct, for example the same part could be tolerance by

- using profile tolerancing (all dimensions are basic) or ...

- using a mix of basic tolerances and geometric tolerances (e.g. 100 +/-0.1 to control the overall length)

My confusion in part comes from not knowing when to use and when not to use the different types of tolerances.

 

[KENAT]

Are you working to ISO - most active members on this forum as ASME and there are some differences.

I forget details but I think perhaps in ISO you can perhaps control location of surfaces with position tolerance but I'm not sure.

As to what to use when, it all comes back to function (at least in the ASME world, ISO may put a bit more emphasis on 'typical ease of manufacture'). Choose which ever scheme makes best use of the available tolerance budget to maximize the number of 'good parts'. Sometimes this is easier said than done though - especially for us non experts.

Posting guidelines faq731-376

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

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

 

[Belanger]

Kenat's right -- I was presuming the ASME Y14.5 rules. In the ISO (GPS) system of GD&T, then position can be used on surfaces.

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

http://www.gdtseminars.com

 

[pmarc]

hobbs101,
In ISO, opposite to ASME, Position can be used to control location of features (i.e. surfaces), however it is rather reserved for nominally flat surfaces. Location of curved surfaces should be controlled by profile tolerances. Therefore I would not recommend applying positional FCF to round hole's surfaces, even if the diameter is basic, but use Profile instead.
For square-like holes Position applied to all flat side walls is absolutely fine.

 

[MechNorth]

Hobbs,
Your questions suggest that you have not yet taken a GD&T course. While everyone here enjoys helping, this isn't the best place to learn the fundamentals of GD&T; there are too many critical aspects and linked concepts to learn here without a good grounding to start with. Unfortunately the standard(s) aren't terribly user-friendly, so you would do well to find a qualified instructor in your area and learn the basics. There are several on this forum, and even some that have posted on this thread. Good luck!

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[hobbs101]

Thank you to everyone for helping me out. It's all a lot clearer now.

MechNorth, you are correct, I haven't been on a course. I bought a book as a crash course when starting a new contract a few years ago. I don't do drafting on a daily basis, so I never really had a proper chance to clarify some of the misunderstandings that I've had (poor excuse I know!). A course would be a great idea and I'm looking in to them in my local area.

Just before I go though, can I just ask one more simple question with regards to the datum reference frame. An ex-colleague of mine told me that datums should always be controlled with respect to each other, e.g. for a basically orthogonal shape, datum A must have a flatness tolerance, datum B must have a perpendicularity tolerance to A, and datum C must have a perpendicularity tolerance to B and C. Is this correct? I've normally just labelled the 3 datums faces as A, B and C with no FCFs. Indeed, when looking through the Krulikowski book it's the same, no FCFs.

The former method makes more sense, but is it necessary?

Thanks in advance.

 

[CheckerHater]

Another “larger than life” question that requires going further into idea of “datum”.

ISO and ASME differ in terminology and number of hoops you must jump thru, so I chose shorter and simpler ASME-leaning explanation that you later may expand using ISO books available.

Basically, datum is imaginary point, line or plane. The surface of your part associated with datum is known as “datum feature”. During manufacturing or inspection process datum features of your part are expected to lean against surfaces of the fixture serving as “datum simulators”.

It is in your best interest that your part fits into the fixture in precise, repeatable manner, but it is not rule chiseled in stone.

So, it is customary to apply some requirements to your datum features, but it is not absolutely necessary – you may apply GD&T to some really rough parts as well.

 

[MechNorth]

Expanding on what C-H posted; EVERYTHING needs to be controlled wrt something higher-order if there is something of a higher-order. Three core steps to GD&T; (1) establish datums (theoretical point, line or plane), (2) control datum features (actual physical feature on the part), (3) locate all features wrt the datum reference frame.
It is very rare that datums are not necessary.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com