Positional tolerance for counter bore and clearance hole

[Sa-Ro]

Deal all

Kindly refer the attachment.

If position tolerance is applied with median plane datum for two holes, is it required to maintain symmetry between holes wrt datum median plane?

If counter bore and clearance hole is mentioned by hole callout, and positional tolerance with MMC condition. MMC will refer to counter bore or clearance hole?

Kindly clarify.

 

[chez311]

What standard are going by, is it ASME Y14.5?

If position tolerance is applied with median plane datum for two holes, is it required to maintain symmetry between holes wrt datum median plane?

No. Symmetry is a totally different requirement (and indeed has been removed in 2018) and is not suggested by a width-shaped datum feature (midplane datum). A position tolerance establishes a tolerance zone basically located/oriented to the the referenced datum features. The features controlled by said position tolerance must fall within the established tolerance zone. There is no requirement for symmetry, other than what may be incidental due to the basic geometry.

If counter bore and clearance hole is mentioned by hole callout, and positional tolerance with MMC condition. MMC will refer to counter bore or clearance hole?

Presumably you are asking how the "bonus tolerance" calculation is affected, and which feature dictates the amount of "bonus tolerance" relative to their respective MMC size. The answer would be both - the single control frame dictates coaxial tolerance zones but it does not mean both axes must fall within the SAME zone. The size of each zone for the counterbore/clearance hole would vary depending on the size of each feature, the only requirement is that they are coaxial.

Though technically the MMC requirement means that the surface interpretation takes precedence which means that both features must simply not violate their individual virtual condition.

To note - the example in your attachment is RFS. I'm not totally clear on the meaning of the questions in that attachment, but they seem to ask about allowed variation based on "measured values" - the axis of the hole and counterbore(s) in that example must both fall within a 0.3 diameter tolerance zone fixed at basic location to |A|B|. Period. This is Regardless of Feature Size or the "measured value" of the position of either hole - there is no requirement for symmetry as stated above.

 

[Sa-Ro]

Thanks for your reply.

from your reply, I understood the following.

Position of one hole will be measure from datum and from that hole, another hole position will measured. Hence no symmetry. If the first hole is at exact position, the second hole can offset for the full geometric tolerance.

Single FCF for coaxial features, each feature will get bonus tolerance wrt the actual size.

Kindly refer my new attachment and provide some more clarity.

 

[Sa-Ro]

attachment

 

[chez311]

You still did not say which standard you are adhering to. I will assume Y14.5-2009 unless you say otherwise.

Position of one hole will be measure from datum and from that hole, another hole position will measured. Hence no symmetry. If the first hole is at exact position, the second hole can offset for the full geometric tolerance.

No. The tolerance zone is constrained only to the referenced datum features. In your initial example both holes must each fall within a 0.3 dia tolerance zone constrained to datum features |A|B|. The position of one hole does not dictate the allowed position of another unless one of those holes is referenced as a datum feature in the position FCF of the other. (Unless we are talking about MMC with unconstrained DOF or datum features referenced at MMB)

Single FCF for coaxial features, each feature will get bonus tolerance wrt the actual size.

Yes.

1) Which method (1 or 2 or 3) is correct and why other methods are wrong?

Methods 1 and 2 are an identical requirement. 3 holds the position of the counterbore more closely to the clearance hole. None are "wrong"* it only depends on your requirements. That said, you have dropped several datum feature references from each feature which I think are missing, unless that truly represents intent (I'd be skeptical of that). It seems to me that the DRF for the central hole position should be |A|B|C|, the position for each hole/counterbore in methods 1/2 (and clearance hole in method 3) should be wrt |A|D| and with either B or C as a clocking datum feature, unless you don't care where the holes are relative to B/C (doubtful). The position tolerance for the central hole and hole/counterbore in methods 1/2 (and clearance hole in 3) could actually be held in simultaneous requirements to |A|B|C| unless you truly need to hole the hole/counterbore to the central hole. The SIM REQT method is usually much cleaner and would prevent you having to decide which B or C to choose as a clocking datum feature**.​

2) Is it possible to define single axis as a datum without affecting the orientation of the holes as displayed?

I don't follow. Please clarify what you mean.​

3) Does the method 2, implies SIMULTANEOUS REQUIREMENT?

Yes, method 2 is subject to simultaneous requirements (SIM REQT). Note this only applies to the position tolerances.​

4) Does the method 3, datum E is simulated from hole 1 for counter bore of hole 1 and datum E is
simulated from hole 2 for counter bore of hole 2?

Not the way you have it drawn - as shown in your attachment datum feature E would be the pattern of 2X holes. See below for a method outlined in the standard to accomplish what you describe.​

*I wouldn't say method 3 is "wrong" per se but I think what you are trying to accomplish is more akin to 7-26 from Y14.5-2009 below. The INDIVIDUALLY requirement creates a separate, individual datum feature for each clearance hole/counterbore pair.

**Edit - it is much more likely as well that the outer profile should be held in reference to the central hole/bolt holes and not the other way around, unless something truly interfaces/mates with B and C. Additionally if that is the case everything could be held in SIM REQT to A. Or the central hole to A, then the central hole designated B and everything else held to |A|B| including the outer profile. Either way, it likely reflects intent better than holding the holes relative to the outside profile.

 

[Sa-Ro]

Sorry

We are refering ASME Y14.5: 2009

 

[Sa-Ro]

Consider my last attachment.

The requirement of dia 20 axis should be centre of rectangle.

The two mounting holes to be position equally away from axis of dia 20 and as shown in drawing - top left one hole and bottom right another hole.

During assembly, the dia 20 will first go inside the mating part bore then the datum A surface will rest at mating part

Two mounting holes will be position to match with mating thread.

I am explaining my understanding about the measurement of GD&T. Correct me if I am wrong

Position tolerance of dia 0.3 wrt B | C for dia 20 boss:

No need to consider datum A.

Because all DOF are arrested except translational towards datum A.

Since we are holding 50 and 30 face, it will not move towards datum A.

Median plan will be derived from 50 length and 30 width. This is our zero point (centre of rectangle).

Now the axis of dia 20 will be measured and it is allowed to offset within dia 0.3.

Position tolerance of dia 0.3 wrt D for dia mounting holes:

Dia 20 will be clamped and datum axis D is established. This is our zero point. (Single axis datum)

Condition 1:
If the hole 1 is measured from this zero point and found exactly at 18 X 8.

Now the hole 2 will be measured from same zero point (learned from your post) and the axis of hole 2 is allowed to offset within dia 0.3.

If the hole 2 axis is at its maximum away (i.e, 0.3/2 = 0.15) 36 X 16 will be 36.15 X 16.15 mm.

Condition 2:
If the hole 1 is measured from this zero point and found at maximum away from datum (i.e,18.15 X 8.15 mm).

Now the hole 2 will be measured from same zero point (learned from your post) and the axis of hole 2 is allowed to offset within dia 0.3

If the hole 2 axis is at its maximum away (i.e, 0.3/2 = 0.15) 36 X 16 will be 36.3 X 16.3 mm

Each hole is allowed to offset dia 0.3 mm wrt datum.

Fig 7-26 is very helpful.

So if I want to position each counter hole wrt the corresponding clearance hole, I have to mention INDIVIDUALLY at clearance hole datum and counter bore geometric tolerance.

Am I right?

 

[drawoh]

Sa-Ro,

I think you are over-complicating the problem. I am guessing that the outline of your part is not critical, and should not be part of your datum structure.

I agree with your datum[ ]A face.

I would specify your centre bored hole pattern as datum[ ]B. This would have a positional tolerance WRT[ ]datum feature[ ]A, which would give you an accurate pattern. I would apply a positional tolerance to your 20mm[ ]diameter, and a sloppy profile tolerance all around the outside rectangle.

An alternate datum scheme would be to use your 20mm[ ]diameter as datum[ ]B, and one outside edge as datum[ ]C to act as a clocking feature. Once again, I would apply a sloppy profile tolerance all around the outside rectangle.

--
JHG

 

[chez311]

During assembly, the dia 20 will first go inside the mating part bore then the datum A surface will rest at mating part

Two mounting holes will be position to match with mating thread.

(...)

No need to consider datum A.

Because all DOF are arrested except translational towards datum A.

This part is presumably bolted together and clamped to the flat face datum feature A due to the bolt preload, correct? And the part may be a tight slip fit (but still with clearance >= 0) to the central 20 dia bore, correct? Unless the part has a interference/press fit to the central bore (and even then it would depend on the amount of interference - the forces involved with bolt preload can be very high indeed), the bolt preload will force the flat face datum feature A into contact with the mating face on the other part.

Consideration of datum feature references requires taking into account the full picture of how the parts mate (including sometimes possible compliance and part rigidity) - not just which features interact or touch "first" during assembly. Unless the assembly condition differs from the above, datum feature A should certainly be considered. You have recognized this in your perpendicularity refinement of the holes to A, so I guess inclusion of A in the position tolerance DRF is not necessary, but it seems incomplete to leave it out. If we assume (z) is perpendicular to A, utilizing A in the DRF allows A to constrain the rotational DOF (u,v) and B constrains (w). Removing A allows B and C to constrain all rotational DOF (u,v,w). I doubt this reflects function. Refer to my edit on my (1 Apr 20 13:18) post for a notes on a few better solutions which would likely more accurately reflect function.


In regards to your "Condition 1/2" its best not to think about it in terms of linear distance to your hole axes - that assumes no orientation error and is a gross oversimplification. The axis of the top left hole must fall within a tolerance zone of 0.3 basically located from your datum features (the actual size of the tolerance zone may change depending on the actual size of the feature). The axis of the bottom right hole must fall within a tolerance zone of 0.3 basically located from your datum features (the actual size of the tolerance zone may change depending on the actual size of the feature).

An even more simple (and technically correct) way of thinking about MMC position is in reference to your Virtual Condition (VC) boundary as the surface interpretation takes precedence. Your top left hole may not violate a VC boundary of diameter 5.5-0-0.3 = 5.2 located at a basic distance from your datum features. Same with the bottom right hand hole.

 

[Sa-Ro]

Drawoh

Our most of the components are like the one attached drawing.

Rectangular RM will be used.

Centre boss feature is sliding fit (0.05mm per side clearance minimum).

The outer edges should not project outside the mating part.

Can you provide your feedback thru drawing representation?

So that I can understand better.

 

[Sa-Ro]

Chez311

The part is clamped with mating part by bolts.

Generally we used to provide 36+/-0.1 X 16+/-0.1 tolerance in both the components.

So worst case the pitch distance is 35.9 X 15.9 in one component.

36.1 X 16.1 in another component.

0.1 X 0.1 axis shift per mounting hole.

Mounting clearance hole is dia 0.3 mm more than bolt dia. So we have 0.1 side clearance between bolt and clearance hole.

Now we want to represent the same with GD&T.

So for +/-0.1 tolerance we arrived dia 0.3 position tolerance and thought that this dia 0.3 tolerance is between holes after zero setting the datum.

What is mean by surface interpretation takes precedence?

 

[drawoh]

Sa-Ro,

It looks to me like your 5.5mm holes are for M5 screws. Your hole tolerances are way more accurate than you require. Let's assume your M5 tapped holes are located from the 20mm diameter with a positional tolerance of 0.2mm[ ]diameter.

Okay, your 20mm sliding fit is a datum feature. You need a clocking feature. You need to contain your outline. You need your screws to fit.

[ul]
[li]Stick with your current datum[ ]A feature, the bottom face.[/li]
[li]Your datum[ ]B feature is your 20mm[ ]H9 diameter. I observe that your tolerance is +0.052/0. The feature is slightly oversized. Is that right?[/li]
[li]I specify your height as 30/29, and I specify it as datum[ ]C. This does your clocking.[/li]
[li]I specify your length as 39, and I make it a basic dimension. I apply a profile tolerance of 1mm at each end WRT |A||B||C(M)|[/li]
[li]Your tapped holes occupy a diameter of 5mm+0.2mm=5.2mm. The clearance hole must not encroach on this. 5.9/5.5[ ]diameter, with a positional tolerance of 0.2mm|A||B||C(M)|. I have left a small safety factor. Note how datum feature[ ]C is a feature of size (FOS).[/li]
[li]I call up your centre-bore a 10.8/10[ ]diameter. The positional tolerance for the hole applies to it too.[/li]
[/ul]

The H13 tolerance you have applied to your 5.5mm hole is +0.18/0. This is a tight tolerance for drilling. Is it really that critical?

--
JHG

 

[chez311]

Sa-Ro,

I think a graphical representation might better explain what I mean. Y14.5 provides us two ways of interpreting position tolerances - in terms of the axis and in terms of the surface. These are called the axis interpretation (or resolved geometry) and surface interpretation. For how this relates to MMC position tolerances you may refer to Y14.5-2009 para 7.3.3.1 - the most common representation you will see is in terms of the axis however this is not the final word. The axis interpretation calculates the allowable axis deviation based on the resulting size of the feature (actually the UAME) ie: for an internal feature at MMC the allowable tolerance zone dia = MMC position tolerance + UAME diameter - MMC size so in your case the maximum allowable tolerance zone diameter is when the UAME=LMC size and 0.3+5.68-5.5 = 0.48 . The surface interpretation establishes a fixed boundary which the feature may not violate ie: for an internal feature at MMC you VC = MMC size - MMC position tolerance so in your case the VC = 5.5-0.3 = 5.2 . These two interpretations will almost never agree as orientation and form error of the feature will create discrepancy (see Figure 3) - hence for MMC/LMC the surface interpretation will take precedence as no matter what the deviation in the axis the requirement is that the feature shall never violate your VC boundary. For an example in the book on how this is calculated see Figure 2.

To put this into perspective for your situation lets take a look at Figure 1. Your maximum linear distance between the two holes is when the feature is at LMC size and offset the maximum amount (calculations I showed above). This is the 39.875 distance I have shown compared to the basic 39.395 distance. We can convert this to x and y coordinates as the below:

basic x = 39.395*cos(23.96) = 36
basic y = 39.395*sin(23.96) = 16

measured x = 39.875*cos(23.96) = 36.438
measured y = 39.875*sin(23.96) = 16.194

The maximum allowable x/y distance between the axes (36.48/16.48) is actually greater but will not exist simultaneously - the maximum x would correspond to a y = 16 and the maximum y would correspond to a x = 36.

These are just clearance holes though. So you're not really concerned about the actual axis deviation - your main concern is that the hole does not cause interference with the fastener. Thats the beauty of MMC, MMC position establishes a VC boundary (aforementioned 5.2 diameter) fixed at basic location which allows more deviation of the feature axis as the size of the feature departs from MMC. As long as the hole satisfies the limits of size and does not violate this VC boundary the feature passes and clearance to your feature is protected.

Fig (1)

Fig (2)

Fig (3)

 

[Sa-Ro]

Drawoh and chez311

Thanks for your wonderful support.

Now I started looking GD&T in correct method.

When I am trying to understand the basic concept of GD&T, I am confused with manufacturing and measurement method.

Why I am considering machining and measurement is, my next stage processor asking doubts. To explain them, I need to be clear from Requirement to measurement.

So there are lots of trailing doubts raised and requesting your patience in advance.

General doubts:

Machining:
If we mention different datum for different features, do the machinist locate / hold the respective datum to manufacture the respective features or hold / locate any one datum and manufacture all features within their respective tolerance zone?

Measurement:
If we mention different datum for different features, do the inspector locate / hold the respective datum to measure the respective features or hold / locate any one datum and measure all features within their respective tolerance zone (like zero setting each time in 2D measurement system)?

What is mean by locate the datum during machining and measurement? It means just touch the datum with datum simulator (If so, it can dislocate during machining or measurement) or touch the datum with datum simulator and clamp?

I am starting from basic concept. (Requirement ----> drawing representation ----> Machining ----> Measurement)

Refer my attachment.

Requirement:
1) The dia 20H9 bore should be assemble into dia 20.1 bore.
2) Mounting screw should be assembled to M5 thread thru Dia 5.5H13 clearance hole.
3) Top plate is not allowed to project outside of bottom plate.

The attached drawing is our regular method of drawing representation. Now we want to define the part thru GD&T for the same requirements.

Let’s discuss step by step procedure:
For requirement 1: dia 20H9 bore should be assemble into dia 20.1

Surface 1 shall be defined as datum A.

The axis of dia 20 boss should be perpendicular to datum A. So that the boss feature and bore will not come to contact.

But the position of dia 20 boss feature is not important wrt datum A.

Drawing representation:
Shall I mention, Perp|dia 0.1|A to dia 20H9 axis without position tolerance?

If position tolerance is required as TP|dia 0.3|A, in what way it will affect my assembly?

If position tolerance is required as TP|dia 0.3|A, For measurement - locate / hold the datum A (translation Z, rotation u, v are arrested) and measure the position from what?.

If gauge is used, dia 20 boss will enter into bore and touch the datum A. But as per the DRP principle, datum must be positioned in the order of FCF. Here before locating the datum, the boss feature entered into the gauge bore.

After I understand this base line, we shall discuss the next step.

 

[drawoh]

Surface 1 shall be defined as datum A.

Good.

The axis of dia 20 boss should be perpendicular to datum A. So that the boss feature and bore will not come to contact.

But the position of dia 20 boss feature is not important wrt datum A.

Drawing representation:
Shall I mention, Perp|dia 0.1|A to dia 20H9 axis without position tolerance?

Yes. There are not yet any X/Y features to position your feature of size from. All you care about is perpendicularity. If you called up a positional tolerance instead of perpendicularity, I believe it would control perpendicularity. It is better to be explicit about this.

If position tolerance is required as TP|dia 0.3|A, in what way it will affect my assembly?

If position tolerance is required as TP|dia 0.3|A, For measurement - locate / hold the datum A (translation Z, rotation u, v are arrested) and measure the position from what?.

If gauge is used, dia 20 boss will enter into bore and touch the datum A. But as per the DRP principle, datum must be positioned in the order of FCF. Here before locating the datum, the boss feature entered into the gauge bore.

I think you need to define your 20mm diameter feature of size as datum[ ]B, locating your part in[ ]X and[ ]Y. There is no need for a positional tolerance. Your position is perfect by definition.

Now, you need a datum feature that prevents rotation. We like to call this a clocking feature.

--
JHG

 

[Sa-Ro]

Now surface 1 is datum A.

Axis of dia 20 boss is perp|dia 0.1|A and defined as datum B.

Any one surface of 50 or 30 shall be datum C -why it is required? No outer surface of rectangle is functional.

Distance between two hole are mentioned as basic 36 X 16.

TP|dia 0.3|B|A|C applied to dia 5.5H13 clearance hole. Axis of dia 5.5 clearance hole as datum D (2X INDIVIDUALLY).

TP|dia 0.1|B|A|D applied to dia 10H13 counter hole (2X INDIVIDUALLY).

TP|0.2|B|A|D applied to 50 X 30 midplane and basic dimension 50 X 30 to ensure the rectangular surfaces are equally separated.

Does two dia 5.5 hole used as datum D or any one to confirm the TP|0.2|B|A|D applied to 50 X 30 midplane.....

 

[drawoh]

Sa-Ro,

A datum feature[ ]C is required because your holes and your outline must be in the same coordinate system. Your 30[±]0.1 width makes a nice feature of size datum[ ]C. You should specify positional tolerances on your holes with respect to |A|B|C|. You can call up |A|B(M)|C(M)|, because datum features[ ]B and[ ]C are features of size, and the tolerances are fairly loose compared to your hole tolerances.

This is the scheme I proposed above (1 Apr 20 18:57). As I noted above, I think most of your tolerances are excessively tight. Based on my Machinery's Handbook, I figure a 5.5mm drill will do a hole between .04 to .14mm over-size. Almost certainly, you want your fabricator to drill your holes. They can get more accurate than drilling, but it will cost you.

--
JHG

 

[Sa-Ro]

Why the datum sequence as A B C for outer rectangle surface?

As per the assembly sequence B A D is right?

Any guidance regarding my general doubt, machining, measurement, datum locate?