TP and FCF basics

[kasabis]

looking in the asme y14.5 1994 pg 53 i see that all TP callouts must have a basic dimension locating these features. If this is true and i am inspecting the part from the example shown, would I have to include the height at which it was measured to have a 3D TP calculation (XYZ), or am I safe in assuming they are only interested in the 2D (XY)location of the hole, and include the -D- datum only as a restrictor to assure the DoF's are locked in in the same fashion prior to measurement?

I know this is remedial but would still like confirmation.
Thanks

 

[caseynick]

Per paragraph 1.4m "Unless otherwise specified all geometric tolerances apply for the full depth, length, and width of a feature." So you need to verifiy the position of the hole at the top, bottom, and everywhere in-between. If the hole is tipped in relation to the primary datum you will end up with different position values at one end and the other.

 

[dingy2]

caseynick is correct.

Dave D.

http://www.qmsi.ca

 

[kasabis]

caseynick, you give me useful information, but as far as the height value included in the calculation, (z axis per se) when this TP is called out, is the third axis a factor?

Do I only inspect/report values of TP based on Basic callouts, or do I include deviatons in the z axis. In other words if I check several "heights" of this hole, do I base my calculations from the 2x(sqrt(dev_X and dev_Y axis) or all three axis

being a feature of size (hole) I know that the mating part must be in the correct X and Y location. It is is the primary datum (which dictates height) that throws my understanding of the calculation off.

 

[caseynick]

There is no z axis deviation. The calculation would be based on the devaition in x and the deviation in y, (at more than one height,z, if the hole is tipped).

 

[Belanger]

Imagine taking a cross-sectional slice at every possible height. The center of each cross-sectional circle must fall within the X-Y position tolerance zone.

John-Paul Belanger
Certified Sr. GD&T Professional

http://www.gdtseminars.com

 

[drawoh]

kasabis,

How are you fixturing your part?

Carefully read Chapter_4 in ASME Y14.5. You should not be measuring from just two edges. Your part should be fixtured so that it cannot move. In such a state, your hole's volume can be defined and verified in three dimensions, as described above.

Read ASME Y14.5M-1994 section_3.4.7 on projected tolerance zones. Better yet, read section_7.4.1 in ASME Y14.5-2009, which goes into more detail. I am not saying your drawings should be done this way. I just think this will make your thinking clearer.

JHG

 

[flash3780]

The tolerance allowance applies to the entire length of the hole (i.e. the top/bottom/middle/etc can move independently within the tolerance zone). The MMC modifier on the positional tolerance allows you to check the part with a functional gage (a go-nogo gage). For this part it will likely be 3 flat surfaces, representing your datums, and two pins representing the virtual condition of the hole at MMC. In addition, a tapered pin would likely be used to verify the hole diameter.

Often, position is used in this way for locating bolt/fastener clearance hole positions. It's a very handy way of making sure everything will fit together. When doing this sort of stackup, you should read up on calculating virtual conditions. Positional error effectively "shrinks" your hole by exactly the amount of the allowable error as far as the bolt that has to pass through it is concerned.

Quick Plug: Parts like this should often be specified as a zero positional tolerance at MMC. This will allow a designer to open up the size tolerance to allow for smaller bolt holes (when better positioned). At the end of the day, it leads to bigger tolerance zones.

 

[drawoh]

...
Quick Plug: Parts like this should often be specified as a zero positional tolerance at MMC. This will allow a designer to open up the size tolerance to allow for smaller bolt holes (when better positioned). At the end of the day, it leads to bigger tolerance zones.

Make sure you set a loose maximum tolerance on the hole diameter. You can figure that a bolt occupies a space equal to its major diameter, and a screw occupies its major diameter plus its positional tolerance. This is your minimum hole size. Add a bit more if you are clamping something thick, or look into projected tolerance zones. Subtract this from your maximum allowable clearance hole and you have your fabricator's error budget. This allows for both the clearance hole's positional error and diameter error. Be reasonable

When the fabricator calls and asks what the f&%k you are doing, answer nicely, and explain the standard.

I love specifying zero positional errors, but I am careful to not make things ultra precise.

JHG

 

[ewh]

I was once called into my supervisors office for using zero @ MMC. The situation did call for tight tolerancing, but it was not an unreasonable requirement. Apparently the project engineer didn't understand how it could be possible, and complained to my boss instead of asking me to explain. When I did try to explain it to them, their eyes just glazed over. I wasn't working for that boss very long. ;-)

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

 

[fsincox]

ewh,
I really feel your pain. My whole experience with GD&T is based on that: "do we really have to use it, "isn't this good enough". I think the people who sell (teach)it do not help the cause by their nods and winks to the management and comments like:
“I really hope that Designers do not use this method since most on the shop floor would not understand it.” ASME GD&T Professional - Technologist and Senior Levels.
I am sorry but this is true of most GD&T if you applied that standard, where are we.
I was once told by a German woman who translated drawing for us that in some factories in Germany the machinists have a pocket chart with tolerances on it and drawings can say "30H13" the shop is expected to know it. Yes to be able to add and subtract, what is wrong with expecting people to be qualified to do their job? I have always wanted to know if this is true. I believe it is the root of our problems now as a country.
drawoh, you are very fortunate to work in a more forward thinking company. That is my main problem with all of these discussions as is almost irrelevant to the way we are actually allowed to work.

 

[drawoh]

fsincox,

Actually, no one at my site is interested in the nitty gritty details of people's drawings. The company is not progressive. I am merely getting away with stuff.

I have only been challenged one by a shop. I explained the standard to them, and they were satisified.

I have a major issue with not using GD&T. According so ASME_Y14.5, anything that appears to be a 90[°]_angle is a 90° angle, ± whatever angle tolerance you specified on your drawing title block. This is very nasty. Take the case that you have a 10"_edge and a nominal angle tolerance of a very reasonable ±0.5°. You have located a hole from this edge to ±.005". What is your maximum error?

ERROR = .005in + (10in)[×]sin(0.5°) = .092in

Your ±.005" tolerance is nearly irrelevant. In practice, machine shops know better than to deliver crap like this, but if they do, you are legally obliged to play for it.

The GD&T standard allows me to specify my holes from a 3D orthogonal coordinate system. Most of the time, I use a profile tolerance to control my part outlines. No GD&T standard, no control.

JHG

 

[dingy2]

fsincox:

As someone you quoted here ("ASME GD&T Professional - Senior and Technologist Levels"), I guess I should respond from my experience but not from a design perspective.

First of all, I have not nodded or winked at management but I have tried to apply GD&T where it enhances the drawing to the feature's function and relationship. Sometimes, one can achieve a certain result by applying a particular symbol that possibly could be easier to understand. Yes, I do suggest that.

My approach is different from most trainers in this subject since the usual approach it to have all dimensions as basic with all surfaces reflected in profiles. Of course, all features of size would be in positonal tolerances too with a +/- tolerance a mortal sin. I still don't understand how that approach enhances the design intent but it sure covers the Designer's butt.

It did take me 10 years of training to be comfortable in this subject but, as this forum reflects, there is still a lot of vagueness out there on this subject. It's complex.

By the way, applying 0 at MMC should not be tough to understand.



Dave D.

http://www.qmsi.ca

 

[KENAT]

No, and yet I got a phone call on it just the other day from someone that actually got to attend the GD&T graining we had here just before I joined (and so got none).

Posting guidelines faq731-376

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

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

 

[Belanger]

A drawing should have something in the notes or title block that says "All dim/tol per ASME Y14.5M-1994" or similar. So when a supplier is contracted to build a part per the drawing, they are obligated to know the proper usage of GD&T. Assuming that the designer uses Y14.5 correctly, the burden is then on the supplier/manufacturer to understand the callouts.

For this reason, I have never said that "I hope designers never use this" in over 15 years of GD&T training. If the folks in the shop can't understand it, another company whose employees can understand it will get the work, so it's in their benefit to learn!

John-Paul Belanger
Certified Sr. GD&T Professional

http://www.gdtseminars.com

 

[dingy2]

J-P:

Yes I do make suggestions when in training.

As an example, I would never suggest using any of the orientation symbols by themselves. Remember, one has to show the location of the feature with a +/-. I would suggest that if a hole(s) is important to the part's function, I would suggest using positional or profile of a surface on surfaces. Orientation symbols are best used for refinements.

If someone asked how one should apply GD&T on a feature, how would you do it? Would you not suggest the best method from your experience?




Dave D.

http://www.qmsi.ca

 

[Belanger]

Hi Dave,
I guess I meant that I don't teach a GD&T tool and then discourage its use. I give them the "toolbox" and yes, I'll provide guidelines and suggestions based on the need of the part and my experience. I'll also give fair warning to designers that some callouts may cause confusion downstream. But I meant that we shouldn't avoid a GD&T symbol or method merely because some folks might not understand it.

As for orientation without location -- it's easily done for a surface feature. Think of a traditional block with a thickness +/- callout, and then parallelism across the top to datum A (which is taken from the bottom surface). The +/- controls the size and the location of the top surface.

For a feature of size, an orientation control can make sense for a hole if that hole is one of the main datums. Think of hole which is datum feature B, and we often use perpendicularity to tie that hole back to the primary datum A. No location needed! But other than that, I would agree.

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

 

[dingy2]

J-P:

I would suggest avoiding concentricity since it absolutely does cause confusion downstream. "Median points of diametrically opposed elements" - figure out how to check that one but I do go over the symbol and its meaning. I would always suggest positonal in RFS or maybe circular runout rather than concentricity.

I do agree that a secondary datum hole can only be qualified to the primary datum with perpendicularity.

I don't believe that I said that I would not use a symbol if some folks would not understand it. I do believe that if a symbol easier to understand, confirm and achieves the same result (such as my example of concentricity), use the easier symbol.

Have a good weekend and PS - December is an awful month for training.



Dave D.

http://www.qmsi.ca

 

[KENAT]

"But I meant that we shouldn't avoid a GD&T symbol or method merely because some folks might not understand it."

While from a design and engineering point of view I really want to agree with you, we for the most part operate in a business world where making money is a priority and so I wonder if sometimes we should temper extreme technical/theoretical correctness if it's highly likely to cause practical problems without corresponding bennefits.

Posting guidelines faq731-376

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

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

 

[Belanger]

OK Kenat, I'll buy that!

Dave -- good point. I too explain the problems of concentricity. But I also try to explain it well enough that if someone does need to use it in its proper understanding, then hey, go ahead. But for concentricity and symmetry those opportunities should be few and far between.

So overall I think we're on the same page.

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