Drawing conversion from plus minus to comply with GDT Std

[SeasonLee]

I am trying to convert a plus minus drawing to GD&T compliant drawing, first page on the attached file is the original plus minus drawing and the 2nd page is GD&T drawing. Here are the changes:

1. Datum setup
* Top surface is primary datum with a flatness control.
* The lower hole is secondary datum and the tertiary datum is the flat portion.

2. Bi-directional position tolerance
1.548±.010 convert to |position|.020m|A|Bm|C|
.928±.015 convert to |position|.030m|A|Bm|C|

3. Profile tolerance
Dimensions on the upper portion from M to N mostly are 2 place decimals; the general tolerance is ±.015, so I will have a large tolerance
|profile|.020|A|B|C|
Dimensions on the lower portion mostly are 3 place decimals, the general tolerance is ±.005, then a small tolerance selected.
|profile|.010|A|B|C|

Questions

1. Can I add a note “Untoleranced dimensions are basic” to simplify the drawing as shown?
2. How to convert an unequal bilateral tolerance .438+.010-.015 to a basic dimension?

Please let me know all my problems and all I missed, thanks for all of your comments.

SeasonLee

 

[dingy2]

SeasonLee:

You are going to be opening up a can of worms for sure here since we have a couple of prevailing concepts on the application of GD&T.

One is to apply GD&T on ALL features whether or not they are needed. One would have default tolerances of both positional and profile of a surface tolerances in notes with maybe a couple of refinement applications directly on the features. Ask yourself if this application will better reflect the design intent of the product.

The other concept is to apply GD&T where it is needed to reflect the features functional requirements. If we have holes that just lighten the product, as an example, their location is not important. Is it better to reflect the holes in positional tolerances at MMC or would the coordinate location with +/- tolerance be satisfactory.

If we have a perimeter of the product that is in space with no functional design requirement, should one place a profile of a surface on this feature or not?

The ASME Y14.5-2009 states in the Forward section vi "it is even more important that the design more precisely state the functional requirements". Does it really reflect the functional requirements having all feature covered by GD&T? The standard does not mandate full coverage.

I remember reviewing a drawing in an automotive supplier. Their Customer told them that they required a default positional and profile of a surface requirement on the drawing. I did notice on the drawing that there was a specific surface with exactly the same profile of a surface tolerance as the default. I asked the Designer why did the drawing have a duplicate requirement and he told me that it was really needed where it was specifically shown on the drawing while the default tolerance didn't really mean anything.

Determine how your company should apply GD&T where the design intent for reflecting functional requirements is best shown.

Dave D.

http://www.qmsi.ca

 

[ewh]

I am in the camp that agrees with Dave. I don't think it is necessary to slather GD&T all over a drawing just to be standard compliant. What the standard does (or attempts to do) is explain the proper useage when GD&T is used. Granted, the use of GD&T may make the cost of fabrication go down, provided the fabricator recognizes any benefit tolerances that may result.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[dingy2]

ewh:

A drawing that does NOT have all features shown in GD&T is still compliant to the newest standard. The standard might recommend a method but it does not mandate it.

How many positional gauges have been made where the holes were just present to lighten the product? How many surfaces were confirmed with a CMM with 1 mm increments when the surface is out in space and only needed a couple of measurements? How much did the supplier increase the cost when all dimensions were covered by GD&T and caused supplier apprehension?

Dave D.

http://www.qmsi.ca

 

[ewh]

Hey, I agree completely!
Others here though may have differing interpretations.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[KENAT]

1. In principle this is allowed, at least in asmeY14.5M-1994 version. I can't remember the exact wording but that probably doesn't matter too much.

2. This will depend on what type of control you are applying to the resultant face or feature (didn't look at the drawing too closely). If a surface profile then you could use .438 and just give an un-equal bilateral surface profile tolerance.

To wade in the issues dingy brought up. A lot of people think you only need to use GD&T for high tolerance/critical areas. To my understanding the standard does not say this is correct, what matters are the actual tolerances whether expressed in GD&T or +-.

However, this widespread belief not only affects how drawings are prepared but how machining the part is costed & performed, inspected etc. Often you can get more expensive quotes for parts converted to GD&t if the machine shop/inspection house etc. don't really understand it. It seems as if some shops add an extra few % for each FCF, even though tolerances have in some cases been relaxed. There have even been threads on this site where fairly experienced people have said they would more closely (hence more cost) inspect a surface defined by profile than one defined by +- even though the tolerances are essentially equivalent.



KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

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

What is Engineering anyway: faq1088-1484

 

[Michael854]

Seasonlee,

I think in the translation, some important concepts have been missed.

The idea of an ASME Y14.5M compliant drawing is to make design, engineering, quality, etc... get the same functional messages from one single master source.

IMO..the most important understanding in translating a drawing from "+/- speak" to "GD&T-speak" is to change implied datum features to explicitly defined datum features.

In doing so...explicitly defined datum feature reference frames should correspond to some kind of function...or at least translate in some way to a function. That way, when the component is checked...the measurement can predict function.

When I look at your drawing, I do not clearly see that ABC corresponds to a function. I see you tried to describe the function by rotation on a theoretical planar datum A...rotation about a theoretical axial datum B....and rotation stopped by a theoretical planar datum C.

However, I don't think datum C will stop rotation in a repeatable manner. The normal vector of a planar rotational stop needs to be tangential rather than radial...and the rotational stop needs to be a sufficient distance away from the axial datum B.

The first question I'd like to ask you is if there is a better choice for the rotational stop datum feature.

I hope this helps.

Michael
GDTP-S0470

 

[dingy2]

Kenat:

You stated "A lot of people think you only need to use GD&T for high tolerance/critical areas. To my understanding the standard does not say this is correct, what matters are the actual tolerances whether expressed in GD&T or +-. ".

You are correct that both the 94 standard and the 2009 standard do not state that GD&T must be applied on high tolerance or critical areas nor does it say that it must be applied to all dimensions in notes. It just doesn't mandate either way but gives suggestions.

I think from a Design perspective, it would be more difficult to apply GD&T where it is needed to reflect "the functional requirements" as stated in the new standard. Just stick default GD&T in notes is much easier but does the end drawing reflect design intent?

I really would like to know why all dimensions should be reflected in GD&T and how does that application "reflect the functional requirements" as stated in the standard?


Dave D.

http://www.qmsi.ca

 

[axym]

ewh,

Yes, others here may have differing interpretations!

SeasonLee,

I like your GD&T drawing. There might be a couple of things on it that need to be tweaked, but it's pretty good. It's already vastly superior to the plus/minus drawing and I don't think any of the GD&T is unnecessary or overkill. Keep doing what you're doing.

I'm wondering about the details of how the part is constrained in assembly or fixturing, that led to Datum B being referenced at MMC. This suggests that Datum B's mating feature is a fixed size and may have some slop, leading to uncertainty as to which datum feature really stops translation in the Y direction - B or C?

Dave,

You're right, this is a can of worms! The anecdotes that you mention are unfortunate, but I don't think that the fact that GD&T was used is the problem. If a company has default tolerances that "don't mean anything", then that is a problem, but it is separate from GD&T. I'm not a fan of block tolerances because they tend to be nonfunctional, whether they're plus/minus or GD&T. If someone is making dedicated gages to inspect lightening holes, then again it's not GD&T that's the problem. Something else has gone wrong in the communication of design intent. The designer probably specified a position tolerance that was much tighter than necessary, or the lightening hole was covered by a default position tolerance just because it was a hole. Possibly the inspection planner thought "it's a position tolerance, I'd better make a gage even if the tolerance is really big" which isn't right either.

Regarding whether or not profile should be used on the perimeter surfaces of a part that are just "in space", i.e. not contacting anything, I say why not use profile? It's not that those surfaces have no functional design requirement - it's just that they don't touch anything. The requirement is that the form and location be close enough to nominal, for other reasons - rigidity, cosmetic appearance, who knows?

I realize that the standard does not mandate that all, or any, features be controlled with GD&T. But the argument that plus/minus dimensions reflect functional requirements better than GD&T seldom holds water, if ever. Take a look at the plus/minus tolerances on SeasonLee's first drawing and see how functional they look. .541 +/- .005 between an imaginary "vertical" line and the imaginary center of a fillet rad? 30 +/- 1 degree between a planar surface and an imaginary "horizontal" line? Functional, I don't think so.

I think that the opposition to GD&T is often a result of a quest to "keep things simple". The designer wants a quick and simple drawing, the manufacturing guy wants simple dimensions to program from, and the inspector wants simple characteristics that can be inspected with hand tools. Plus/minus tolerancing satisfies all of these things. This works fine for certain parts, where the form and orientation error of the features is small compared to the location tolerances that are required.

But on a piece of formed sheet metal like SeasonLee's part, things are not that simple. Those plus/minus dimensions and angles are a nightmare to inspect in a repeatable way on sheet metal, believe me I know. It doesn't matter if hand tools are used or if a CMM is used - the linear distances and angles become ambiguous on a real part with form error. This is why we have GD&T, for parts like this!

Once the hope for "simple" hand tool inspection is abandoned, and coordinate measurement technology is embraced, GD&T is generally much easier to inspect. If I were the CMM programmer, I would take SeasonLee's GD&T drawing over the plus/minus version in a heartbeat.

I think that one of the main reasons for "supplier apprehension" and accompanying cost increases is that they won't be able to measure the parts with just calipers and a protractor. If this is a limitation that the designer is forced to work within, then making a GD&T drawing won't add any value.

Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca

 

[SeasonLee]

Dave and ewh

Thanks for your inputs. Definitely I agree all you said, reflecting functional requirement is the major consideration on a GD&T print, but for this part I will think more about the manufacturing process and its inspection.
It’s a casted part with a small hole Ø.180, then a secondary machining to ream the hole to the specified hole size Ø.190+.005-.000 (since they worry about the casting can’t meet a only .005 tolerance hole size), they use this hole as a guide to locate the part and drill the other hole, that’s the reason I am choosing the lower guide hole as secondary datum.
I am always facing the questions from manufacturer: How do you setup the datum on your dimension measurement? It’s my intent to convert from implied datum to explicitly defined datum, both manufacturer and we will have a same measuring datum to reduce any potential argument.
Frankly speaking, the drawing conversion is on the view point of manufacturing and inspection, the end user will take our drawing as a reference to update their own drawing accordingly.

Dave

Would you please advise the general default positional and profile tolerance on a part design.

Michael

I can understand your concern, if datum C will not stop rotation in a repeatable manner, can I choose the two holes as a pattern to establish the DRF?

Even

Thanks for your valuable comments

SeasonLee

 

[ewh]

Those are indeed valid reasons to convert. The result is a much easier to understand part definition, and should ensure that the resulting parts will meet their design intent.
To be honest, I didn't even look at the drawing when I made my comment; I was just attempting to point out that (IMO)just because a drawing doesn't contain GD&T doesn't mean it is not a valid drawing per the standard. I am not in the least opposed to applying GD&T, and make no claim that +/- dimensioning better defines functional requirements. I recommend and prefer to use GD&T vs +/- dimensioning. I just have a problem with stating that a drawing must contain GD&T to be valid per the standard.
Evan's post contains an excellent explanation of how to approach your situation and why.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[dingy2]

SeasonLee:

Sorry but I would not recommend the use of a default positional and profile tolerance on a drawing. I would leave the default co-ordinate tolerance already established alone and apply GD&T where you need it.

I would suggest that the face of the part should be the primary datum (could qualify with a flatness tolerance) while one .190 hole would be the secondary (all dimensions come from here) and the tertiary is the other .190 hole. Since this is a stamping, the secondary can only be qualified with a perpendicularity tolerance and that would not be a problem so I would just designate the hole as a secondary datum. The tertiary hole could be qualified from the primary and secondary using a positional requirement.

Now you are ready to apply GD&T where it might be needed.



Dave D.

http://www.qmsi.ca

 

[dingy2]

GD&T is much better at defining functional features and should be used. I have never stated that +/- are better on functional features.

Dave D.

http://www.qmsi.ca

 

[fcsuper]

Having a general profile tol is useful if you have a model and use it as completely basic. However, orientation comes into play and should be considered.

I cannot think of any situation where a generic positional could be use for parts that are more complex than a simple plate. Orientation would be a major concern since you'll be forcing the both fabricator and inspectors to be handle the part in multiple set ups that may not fall in line with the function of the part.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

 

[SDETERS]

Why add a note for the basic dimensions. Show them basic and be done with it. I can not imagine taking it that much time to make each dimension basic.

Questions on the drawing?

1. Why have a flatness .010 you already have this with your default tolerance .313+/-.005. What are you trying to do with this call out?

2. If you do put on your drawing the note for basic dimensions make sure your number of decimal places match the number of decimal places in the FCS block it goes back to.

3. What is your tolerance for the b datum back to a datum?

Thanks

 

[SeasonLee]

Thanks for all of your inputs, the attached drawing revised, changes made are:

1. Unequal bilateral tolerance .438+.010-.015 changed to .438, it will cover with the profile tolerance |profile|.020|A|B|C| which is equivalent to ±.010, a little tighter than the original tolerance.

2. Point N moved to the right end.

3. The other hole designated as tertiary datum C.

4. Bi-directional position tolerance changed to |Postion|Ø.028m|A|Bm| which is equivalent to ±.010, a little tighter than the original rectangle tolerance zone.

5. Datum B as a dimension original point and all dimensions changed to ordinate.

SDETERS
You are right, the original thickness tolerance is ±.010, it was deleted accidentally.

Now, the other hole designated as tertiary datum C, there will be no more rotation stopped in a repeatable concern, it’s easy to make a change on a CAD software, but here I am thinking how to setup the X-axis (or Y-axis) on CMM measuring, your help will be highly appreciated.

Again, need your comments to pinpoint all I missed.
Thanks

SeasonLee

 

[KENAT]

Season Lee - back in the office and have my std to hand.

1. Per the 94 version page 81, 5.2.1.1 "UNTOLERANCED DIMENSIONS LOCATING TRUE POSITION ARE BASIC" is the phrase.

2.Take a look at 6.5.1(b) & figure 6-11 for "Bilateral tolerance unequal distribution", or have you decided to tighten it based on function?

dingy, I think you've misunderstood me. I'm hesitant about all over or default surface profile or position tolerances, except possibly for some MBD applications.

I also don't believe that all dimensions/tolerances should necessarily GD&T. I believe it should be driven by function and expressed per the relevant standard.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

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

What is Engineering anyway: faq1088-1484

 

[SDETERS]

If this is case "UNTOLERANCED DIMENSIONS LOCATING TRUE POSITION ARE BASIC" What bout the dimensions that are defining the Pofile of surface on the drawing? I just do not like this note. Show the dimensions being basic for clarity reasons. It is not that hard to do so.

 

[KENAT]

SDETERS, I had the same thought when I first read it, in the case where there are surface profiles as well it should arguably be "UNTOLERANCED DIMENSIONS LOCATING TRUE POSITION OR TRUE PROFILE ARE BASIC".

I don't particularly like it, and don't use it, but it is perfectly legal to the 94 standard.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

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

What is Engineering anyway: faq1088-1484

 

[SDETERS]

Ok I agree with that. If that is acceptable practice for the company on the way they to do things and that is cool.