Simple plate

[PRuggiero]

Had a simple question, I think.

Imagine I had a plate with four holes in it, don't really care about the perimeter of the plate, just the position of the four holes relative to each other.

Currently I have the bottom of the plate as datum A and the far left hole datum B (with a perp. tolerance of .005 to datum A). I then have the other three holes as a 3X XX.XX" with a positional tolerance of .005 to A and B.

After reading on here about how it is common to GD&T a little more than necessary I started thinking...

Could I just have a positional tolerance for all four holes .005 relative to datum A and achieve the same thing? 4X XX.XX" with the GD&T block right under that call out. Any advantage to one way or the other?

 

[fsincox]

Basically, yes, I would actually say the prefered thing if they are all a single pattern used for the same thing. What you proposed can be done but it really confuses the issue as it makes one hole look more important that the others. If that is true determined by functional requirements then there may be a good reason. Say (2) are dowel holes and (2) are clearance fastener holes. Also, I believe it is the same if all features and the datum hole was to be referenced at MMC/MMB.
Frank

 

[CheckerHater]

PRuggiero,
You just explained in this thread -

http://www.eng-tips.com/viewthread.cfm?qid=315731

- what will it take for operator to start drilling the holes, so you still have to throw in some dimensions to tie holes to the edges of the part.
And Frank, (and we are threading thin ice here) what is your favorite method to identify dimensions one doesn't care about much?

 

[fsincox]

CH,
Why thin ice? In this case?

PRuggoiero (don't do what follows if it does not meet the funtional requirements!!!)

CH,
simple machined part: position (4) holes to datum A, profile outside to a number that can be checked with a tape measure, say .060? I might include the pattern as datum on the profile if needed. Maybe the opposed face parallel to datum A. Note: "all dinensions basic".

That is what I believe will send the best message to a trained GD&T manufacturing person. I have a block with (4) holes that have to be good within ..., the outside I don't care about much!
Frank

 

[KENAT]

Well, you could do something crazy like make the pattern of holes itself the secondary datum and then tie the edges of the part to that datum. Which now I reread it is an option fsincox mentions.

Posting guidelines faq731-376

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

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

 

[lisa247]

Unless i've read this wrong, if you position all 4 holes 0.005 relative to datum A, how are you controlling the position of the holes relative to one another? Or are you suggesting that you make one of the hole centres datum A instead? I would say your original method is the best way to achieve what you are trying to achieve.

 

[KENAT]

Lisa, if all 4 holes have the same call out then they get treated as a pattern with 'simultaneous requirements'. They already have basic dims between each hole, and if the orientation is at 90° you get to assume basic 90°. So the holes are adequately defined to each other.

What the OP doesn't mention but fsincox and I then touch on, is how you then relate the edges to the hole pattern.

(Section 4.5.8 of Y14.5M-1994 talks of pattern of features as datum, while 4.5.12 addresses simultaneous requirements.)

P.S. I've assumed ASME stds, which might not be correct.

Posting guidelines faq731-376

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

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

 

[fsincox]

Lisa,
The position tolerance controls the holes relative to on another, it always has.
Ken is correct, If the simultaneous requirement is not sufficient, I am not a strong supporter of it myself, I would state the pattern as a datum.

I believe ASME Y14.5, fig 4.26 was actually developed fron my discussions with members of the committee and the gearbox examples we showed them. If this was not the case it showed me others had the same concerns, then. I certainly see the similarity, although much simplified.
Frank

 

[fsincox]

Remember, I was asked what is my prefered, I did not say if fits this function or even more that "your" checker will let you get away with it. Ours fought it tooth and nail, at the time, I am the checker now!
Frank

 

[lisa247]

But what PRuggiero said was

'Could I just have a positional tolerance for all four holes .005 relative to datum A and achieve the same thing?'

If datum A is the flat surface that the holes are to be drilled through, how can you state that you want the holes to be drilled within a positional tolerance relative to datum A? WOuld you not state your perpendicularity relative to datum A? Does there not need to be a datum B to measure the positional tolerance against? I've not studied GD&T for a while so maybe this is just my lack of practice becoming evident.....

 

[CheckerHater]

Frank,
This is exactly what I wanted to know - you'd prefer all-around profile using hole pattern as a datum, right?
Other options being composite position to 2 edges; width and height as datums of size in case of symmetrical plate; combining basic and directly toleranced dimensions, which is still "not recommended" but not explicitly forbidden; and... what else?
I like profile for the edge, but I am scared by tales of non-GD&T trained estimator adding 5% for every FCF. Any other option will have its own drawback. All of them were subject of heated discussions before, hence "thin ice".
Just trying to collect personal opinion, that's all.

 

[fsincox]

Lisa,
You are fine; your thinking is VERY conventional. The position tolerance holds the holes together and a number like .XXX (should be an actual calculated value!!!) tells everyone these holes must be held together AND perpendicular to datum A.
The key is we don't need to follow process and when we do WE get burned, they will change the method they want to use and we will be wrong again. We follow function that is what we know, they do not! In 10 years when all parts are made by stereolithography the edges will not matter much.
I had an old GD&T instructor once tell me: "tell them to think of it like a football field" If I tell them it must be 100 yards from one end to the other, which end they want to start with is their business. Profile says it must be .060 (or whatever you want) from the holes to the edge, if you start at the edge so be it, start anywhere you want. The number should be such that the guy in the shop says I can hit that blindfolded on a bad day. As the ISO says to give him more tolerance is useless.
Frank

 

[KENAT]

Lisa, the position tol still applies to the location of the holes relative to each other, not just to some global datum reference frame.

Posting guidelines faq731-376

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

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

 

[fsincox]

CH,
I understand completely, I am talking a world where people are educated in GD&T and take it seriously not just view it as a hindrance, or to put it another way when it is used as it is intended, not just conventionally. The 2009 standard "FOREWORD" lays out some of this vision.
Frank

 

[lisa247]

KENAT, I understood that, I just didn't realise that you could specify a positional tolerance relative to a surface.

 

[fsincox]

Lisa,
With a pattern of holes absolutely, with a single hole, the validity of using a position callout to specify simple perpendicularity is being discussed in the following thread NOW!
thread1103-314972
Frank

 

[KENAT]

Ok, so Lisa the datum reference is for perpendicularity, which I think you'd already brought up.

Posting guidelines faq731-376

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

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

 

[PRuggiero]

I will have to read up more on the simultaneous requirements in the spec. I correct to say that is the only reason why I am able to do just do a positional tolerance for all four holes relative to A and it will also apply relative to the holes too?

I thought I remember seeing a video on the reasoning behind that simultaneous requirement and they explained it by showing a fixture that would be used to check a part like mine. The pins on the fixture used to check the holes were all present thus it requires all the holes to be relative to each other. But what is keeping one from having a fixture with movable pins? That fixture could take care of the perp. tolerance without requiring the pins be relative to each other.

 

[fsincox]

Yes, It will apply to the intra-pattern relationship, too.
You can use the sides, most would, it is VERY conventional. A position tolerance applies to the pattern of holes, when specified as such, by a convention like 4X ..... (position tolerance). Another conventional way would be to use a composite position tolerance to keep the holes together as a pattern tighter than the pattern of holes to the sides, that very well might serve you.
I have a fundamental philosophical issue with implying one set of sides is more important than the other, if they are NOT! Other people will make that very conventional choice all of the time! There is no reason for you to go looking for trouble. I'll take care of that
Frank

 

[lisa247]

thanks fsincox, very informative.