+/- Tolerance vs GD&T 1

[Sa-Ro]

Hi

Refer attachment.

My doubt:
1) In +/- tolerance method, the maximum possible displacement is 20.1 / 19.9.

2) In GD&T method, if the hole 1 is produced at exact 15 (though dia 0.1 position tolerance available), and the hole 2
produced at maximum tolerance (i.e, 0.05 away or towards hole 1). Hence the maximum possible dislocation is 20.05 / 19.95.

3) Hence the tolerance in GD&T is 0.05 less than +/- tolerance method.

4) Is there any other method, to utilize unused 0.05 tolerance from hole 1.
Consider there are "n" number of holes to be produced horizontally.

 

[3DDave]

OK, so RFS on both features it is. I thought you were looking to maximize the error.

 

[Sa-Ro]

@ Drawoh

Nice article.

 

[Sa-Ro]

@ 3DDave

Yes. RFS and RMB condition.

I don't want to maximize the error. Trying to utilize the unused tolerance.

 

[3DDave]

So, what device is this important for?

 

[Sa-Ro]

It is used in a pneumatic product assembly. Locating pins (Placed at 20 basic) will enter into this hole.

Position tolerance may be applied to the functional requirement.

During the GD&T notation, utilization of unused tolerance doubt raised.

 

[chez311]

I don't understand this line.

To put it simply, I WOULD expect on a part produced on a CNC that the horizontal location of the nth hole is within (20*n) +/-0.1 from the first hole which is allowed by the position tolerance with basic dimensions (for n=10 within 200+/-0.1) and NOT (20.1*(n-1)+20)+/-0.1 from the first hole which is allowed by the +/- directly toleranced location (for n=10 within 200.9+/-0.1). I do not envision the "unused tolerance" you are concerned about would really be used. This is just due to the fact that the errors in a precision machine tool do not stack like that if done in a single setup. If you were re-fixturing for every single hole, especially in a manual process, this might be a concern.

In addition to not being very beneficial to manufacturing, besides perhaps giving them the excuse to produce very sloppy parts, I am as skeptical as others here about how this concern about unused tolerance translates into a functional requirement in the actual assembly. Say an n-number of pins on one part go into n-number of holes on another part simultaneously (ie: all pins are fitted to all holes at the same time). What you are asking to replicate the directly +/- toleranced case to allow the first and last pin to be either 20.1*n or 19.9*n away from each other could easily lead to two parts which cannot assemble*.

It is used in a pneumatic product assembly. Locating pins (Placed at 20 basic) will enter into this hole.

How do these pins mate with the assembly?

*that is, if manufacturing ended up producing one part with first and last pins of separation 20.1*n and a mating part with first and last hole of separation 19.9*n.

 

[Sa-Ro]

@ Chez311

I agree that nth hole will offset in +/- tolerance method.

So I am using position tolerance. No doubt in that.

For discussion purpose only....

Consider only two hole to be produced at 20 +/-0.1 between distance, RFS, RMB condition.

How to establish?

 

[drawoh]

It is used in a pneumatic product assembly. Locating pins (Placed at 20 basic) will enter into this hole.

The standard practise for locating on pins is for one of your holes to be a slot. This way, your tolerances reflect only how repeatably you want to locate your plate.

Let's be silly and locate your plate with two round holes over the pins. Assume the pins have a maximum size of 10.1mm. We use true position tolerances of 0.1mm[ ]DIA. The pins are a secondary datum feature with the following FCF...

|<pos>|<dia>0.1|A|

This FCF is tagged as datum feature[&nbsp;]B.

Your clearance holes also are a secondary datum feature. If your holes clear your pins, they must keep out of the space defined by MMB of the holes, plus the true position.

Clear space = 10.1mm + 0.1mm = 10.2mm.

Clear space, plus the true position of your holes defines the MMB of your holes...

MMB of holes = 10.2mm + 0.1mm = 10.3mm.

<dia>10.5/10.3
|<pos>|<dia>0.1(M)|A|

Alternately, you can go...

<dia>10.5/10.2
|<pos>|<dia>0(M)|A|

Note how I did not change the LMB hole diameter. This give your fabricator to work more accurately if they can do a true position more accurate than 0.1mm.

A hole and slot definitely is the better way.




--
JHG

 

[Sa-Ro]

Yes. I agree.

hole for location and slot for orientation

 

[Burunduk]

Sa-Ro,
Considering you said the function of the holes is to mate with pins in a pneumatic product assembly, I am curious why the distance in the horizontal direction not being more than 20.1 was stated as the design requirement?
Note that the "horizontal" distance is not necessarily the total spacing between the axes - there can be a "vertical" component which is allowed by the way the part is dimensioned with the +/- tolerances, producing a total distance of more than 20.1 between the axes (and I'm making an assumption here that the axes are produced parallel and the distance is measurable).

So could you address why the horizontal direction more important than any other direction, and what defines this direction without datum features specified? I am interested in the reasoning that was applied to drive this design requirement.

 

[Sa-Ro]

@ Burunduk

design requirement is not only in horizontal direction.

For my understanding, I have limited the discussion to horizontal direction only.

Though the location of the hole can be benefited from position tolerance, I just compared the RFS and RMB situation with +/- tolerance (To utilize the unused 0.05 tolerance from hole 1 as said in earlier post).

 

[Burunduk]

Sa-Ro,
What locates the part in the assembly? You said it mates with locating pins, so I assume the part is not located by datum features C and B as in the option that shows what you call the "GD&T method", is that right? If so, your datum reference frame should be reconsidered and you shouldn't even care about the location of the first hole relative to the edges of the part to determine the allowed position error for the second hole. Therefore the "unused tolerance" you mention is probably not what you should be thinking about.

 

[Sa-Ro]

You are right. Datum B and C are not locating the part.

Let's forget the datums. Consider two holes only.

Between centre is 20 +/-0.1.

Both the holes are dia 0.1 position tolerance allowed. Hence 0.05 per side per hole.

If hole 1 is produced at exact location, the hole 2 can shift by 0.1 which will violate 0.05 per side position tolerance.

Without FCF method, the hole can shift by 0.1.

 

[chez311]

If only located to A and we are only talking about two holes, the two holes can be at 20.1 separation even with the FCF position tolerance no matter where either hole comes in at.

 

[Burunduk]

Sa-Ro,
I agree with chez311.
With position tolerance to A within 0.1 applied on a pattern of two holes, you have two 0.1 diameter cylindrical tolerance zones perpendicular to A with their centers spaced exactly 20 apart. The axes of your two holes can fall anywhere within these tolerance zones. The maximum spacing is 20.1 and the minimum spacing is 19.9.

 

[Sa-Ro]

Correct. I understand that very well.

But, read my last post.

If hole 1 is produced at exact location, the hole 2 can shift only by 0.05 from true position - either side.

 

[Sa-Ro]

This is what I meant.

 

[chez311]

Your tolerance zones are not location constrained to any datum features. The tolerance zones you show in your figure could shift another 0.05 to the right.

 

[Sa-Ro]

Kindly refer my first attachment. There are datums defined.

Hole 1 and 2 is located from datums.

In my last post I have shown only tolerance zone.

 

[Burunduk]

If hole 1 is produced at exact location...

Although you said "forget about datums", it is important to know what kind of position control you have in mind. Do you agree with the suggestion that since the 2 holes are the features that locate the part, the position control applied to them should only reference datum A? If yes, the location of the first hole is irrelevant because it is only constrained in orientation by the referenced datum. If the holes are produced spaced 20.1 apart, you can still approve the part by finding the "best fit" between the actual axes and the two tolerance zones. Nothing makes you keep the first hole centered on its tolerance zone cylinder.

Anyway if what you care about is the Min/Max separation of the axes and not just in the horizontal direction, the direct tolerances do not give you any useful extra tolerance. Not of the kind that is able to keep bad parts from being accepted.
By the way, there is something wrong with the "Tolerance zone" in your drawing. The square that inscribes the 0.1 diameter should be 0.1X0.1, not 0.2X0.2.