ISO Position GD&T and Dimensioning Questions 4

[Jieve]

Hello guys,

I have a number of GD&T and Dimensioning questions for you as I’ve been working on drawings to send to our shop. I am working to ISO.

1)If a hole is located at the center of a rectangular part, is it necessary to dimension the hole from the edges? I thought I read somewhere that where no dimensions are drawn, symmetry is assumed.

2)Modification of question 1: I have a rectangular part with two holes evenly spaced about the midplane. The hole are also equidistant from the edges of the part. Is it ok to simply dimension the distance between the holes, without dimensioning from the part edges? If so, is it necessary to include a centerline (or centerplane) to indicate that this symmetry assumption is correct under ISO?

3)I have a rectangular plate with a hole in the center. I would like to add a position tolerance to keep the hole within 0.1mm from the exact center. I am assuming that the best method be to make the midplanes of the part datums B & C (with the primary A being the surface the part sits on), and then specify that the position tolerance should be relative to A,B,C rather than making the edges of the part the secondary and tertiary datums? Am I correct?

4)I am somewhat confused about the use of basic dimensions. Assume I have a rectangular part with two holes spaced equidistant from the centerplane of the part. The actual distance between the holes is more important than the distance between any edge and any hole. In one scenario, I make the flat surface on which the part sits primary datum A, and each perpendicular midplane datums B & C. I specify a position tolerance of the first hole from datums A, B and C. Then I make the first hole datum D, and specify a position tolerance of the second hole relative to A, D, B. There is still assumed symmetry of the holes about the midplane. Is it required to specify basic dimensions to the edges B & C to the first hole, even though symmetry is assumed?

5)An extension to question 4, if I use a centerplane as a datum, is it necessary to add basic dimensions from the midplane to the hole?

6)I have seen another example where the part in question 4 had only datums A, B & C as described. One hole was dimensioned with basic dimensions from datums B & C, and the second hole was dimensioned from the first hole with a basic dimension as well. Both had a position tolerance with respect to A, B & C. I thought that this essentially means that both hole dimensions need to be inspected with respect to datums A, B & C, and not with regard to each other. When not using GD&T, when the position between two holes is important, the distance between holes should be dimensioned directly to eliminate tolerance stack-up. But what is the relevance of dimensioning between holes in this case when the datums (i.e. measurement locations) are specified as edges? Would it not have made sense for them to have dimensioned both holes with basic dimensions from the datums? This example was in an ASME book.

7)This may seem like a repeat question of one or two of the above, but assume I have a hole in a rectangular part. That hole has a position tolerance from datum B, which is the edge of the part. Can I use a basic dimension from the opposite edge of the part, or does it need to be from the datum edge?

8)I have 4 holes in a rectangular pattern on a rectangular part. Datum A is the flat surface the part rests on, and datums B & C are the other 2 perpendicular part edges. Each hole has position tolerances. One hole has a dimension callout 4x and the diameter. A position control frame is placed underneath this. All holes are the same size, but not all have the same position tolerance. Therefore, I use a position control separately on the other holes with deviating geometric controls. Is the 4x the diameter callout with the position control frame underneath OK even though the geometric tolerances are different on different holes?

9)Extension to question 8, except now datum D is one of the holes. I specify the position tolerance of another hole relative to frame A, D, B, where B is one of the sides. What distance would be measured upon inspection, the distance from datum D or from datum B? B is really only used to eliminate rotation in this case.

I know these are a lot of questions, but all questions I came across today while working on drawings. Your insight and help would really be appreciated, as always!

Thanks!!

 

[pmarc]

It is a lot, but I'll try:
1. If width of plate serves as a datum feature, so the datum is its center plane, there is no need to give basic dimension for hole's true position. 0 basic dimension is implied. If however datum is derived from the side wall of the plate, basic dimension is necessary. This applies for ASME as well as for ISO.

2. Again it depends on which feature is datum feature. If plate's width, then the basic dimension between holes center is sufficient. If side wall, then you need basic dimension tying one of the holes with datum side plane.

3. It is a matter of functional requirements. Datum features should be selected mainly based on mating relationship of the part with other components in assembly. Both scenarios are reasonable depending on application. So it shouldn't be said that in general one option is always better than the other.

4. If you were working according to Y14.5, then I would say composite positional tolerancing should be your choice to solve this particular dillemma. Upper segment would control location of the pattern, while lower would tighten holes spacing. In ISO GD&T there is no such thing like ASME's composite positional tolerancing. You can use the method you described, or use two single segment position callouts (first with A|B|C referenced, second with A only or A|B). You just have to remember that when calculating maximum and/or minimum possible distance between the holes in both scenarios, the results will be different.

5. No, it is not necessary, though in my opinion placing 2 basic dimensions for each hole from the center plane instead of putting only one basic dim. between holes axes is more transparent.

6. The way how the holes are dimensioned with the use of basic dimensions - whether both from side walls or one from the side wall and the other from the first one - does not matter. Basic dimensions are theoretically exact, meaning they have no tolerances, so they are non-cummulative. They serve to define true (ideal) location of positional tolerance zones with respect to certain datums. As long as there is a path of basic dimensions that enables finding true position of each tolerance zone, everything is absolutely correct.

7. As long as dimension for width of the plate is not basic, you should not dimension hole's center from the opposite-to-datum-B side of the plate.

8. I think it is acceptable. Imagine what would happen if there was 30 holes for example insted of 4. Would you put 30 diameter dimensions for each hole separately? I do not think so.

9. Distance from D should be measured. Or to be more precise, positional deviation (error) of hole's axis from its true position located at a certain basic distance from datum axis D. Datum B serves for constraining rotation of the part only.

 

[fsincox]

Good job, pmarc,

NO COMPOSITES in ISO, wow! How did I miss that! I knew there were things I liked in ASME better.
Frank

 

[Jieve]

Pmarc,

Thanks so much for answering all of those questions so clearly! I'm so thankful for you taking the time to help me out. I had just read about and was in the process of adding a composite position tolerance to a hole pattern when I read your post. I therefore added a refinement tolerance as you mentioned. A couple more questions:

1) Assume I have a rectangular flat part with a 4 hole pattern. The primary datum is the flat face upon which the plate is laying, the secondary and tertiary datums are two other perpendicular edge faces. I add a position control below the 4x hole designation, which then applies position tolerance zones to each of the four holes. I then wish to refine this tolerance, limiting the movement of the tolerance zones relative only to datum C. In the refinement control, am I still required to specify the control relative to datum A if I am not interested in increasing the perpendicularity tolerance, or can I simply leave datum C as the only datum in the refined control frame? I recently read that ASME requires including the datums in the refinement frame in the same order as in the original control frame.

2) Assume I have the same rectangular part but only with a hole in the center. The datums are now the flat face on which it rests, and the perpendicular midplanes. I have a hole in the center, but I do not use any position control on the hole. Since this hole is not geometrically controlled, is it still necessary to add a dimension from the edges, or is it still assumed to be in the center because the datums are midplanes, even if there is no position control used?

3) Assume I have a circular disc with a hole through the center. The primary datum is one face of the disc, and the secondary datum is the center axis, specified by attaching the datum symbol to the dimension of the outer diameter of the disc. I want to control the concentricity of the inner hole to the outer diameter, so I add a position control to the center hole relative to both datums A (face) and B (axis). Since I have an angular title block tolerance of +-1 degree, I want to also limit the angular deviation of the outer edges of the disc, so I specify a perpendicularity tolerance added to the dimension of the outer diameter of the wheel (where datum B is attached). The perpendicularity tolerance is therefore valid for the center axis of this feature. However, the position of the center hole controls the perpendicularity of the same shared axis. I am assuming it is still necessary to have both of these controls to achieve my stated goal. Am I correct? Or does one control on that axis satisfy both conditions?

4) Assume I have the same disc, this time with 12 holes spaced 30 degrees apart from each other equidistant from the center point. I have another set of 6 holes closer to the center, this time spaced 60 degrees apart and also equidistant from the center. However, the second set of holes is offset from the first set of holes by 15 degrees. All holes are the same size. I specify a position tolerance on the holes relative to the flat face and center datum axis, saying that their center axes can only deviate 0.1mm from their exact centers. I then make the diameter dimensions and angle dimensions that locate the holes basic. Since there is an angle dimension between holes, am I required to add an extra clocking datum to the part? If so, would it be best to use the center axis of one of the outer holes as that datum?

5) I have a part that will be made out of aluminum angle 90 degree profile, which will most likely be cut to length using a band saw. The length tolerance is not important for the function, it is therefore left to the title block tolerance of ISO 2768-m. However, I would like the edges cleaned up, smooth and straight. Would it be better to simply specify perpendicularity controls on both ends, or should some other combination of flatness controls or surface finish callouts be used? If a surface finish, what would you recommend?

Thanks so much for all of the answers, Pmarc if you were here, I'd owe you at least a couple lunches for all of this.

Thanks!

 

[pmarc]

Jieve,
First of all, thanks a lot for those really kind words. I guess that in this case I owe hundreds of lunches to all of those who helped me here on this forum throughout my membership. It is not that I have always been on the side where I am know. I started just like you, by asking questions - sometimes very fundamental (even silly), sometimes slightly more complicated. The most important thing was and still is that I wanted to learn more and more. That is why I really like your attitude - it is clear from your very first post (at least to me) that you are eager to learn GD&T fundamentals too. I hope this will not change quickly.

Okay, but back to main topic...

1. Shortly saying you do not need to repeat datum A in second feature control frame, although I would recommend keeping A untouched. For sure it will not make you situation more complicated. The thing you mentioned about ASME applies to composite positional tolerancing (one common position symbol for both FCF segments). Since for ISO GD&T such callouts are not standardized (and even if used, they have the same meaning like two single segment FCFs), you are allowed to specify whatever datum(s) in the second FCF. Those could be even completely different datums. For your particular application I would suggest referring to |A|B|C| in 1st FCF and refine it by |A|C| in 2nd FCF.

2. Here your are touching very questionable concept which is well known and commonly used in ISO world, but has been really criticized by many ASME folks. It is the idea of general geometrical tolerances. (I am not calling myself ISO or ASME guy, rather ISO/ASME hybrid, but I also have a lot against this concept). The fact that you are not showing any geometrical tolerances for hole does not have to automatically mean the tolerance is not there. If your print refers to ISO 2768, it is understood that general symmetry tolerance between datum B or C and hole's axis is applied. Knowing this, you do not have to specify any dimension from the side of the plate or from its center - implied 0 basic dimension is already in, and the maximum allowable error is defined in Table 3 of ISO 2768-2:1989 depending on tolerance class and lengths of considered features.

3. You are assuming correctly - those 2 callouts (position and perpendicularity) do not exclude each other. As a matter of fact this is how GD&T shall be applied in such cases. First choose primary datum feature (bottom surface), then pick a secondary datum feature (cylinder) and control its orientation (perpendicularity) to datum plane A derived from datum feature A. After all of that, control position of the center hole to datum reference frame |A|B|.

4. You do not have to add any tertiary datum to those callouts in order to keep mutual angular relationship between patterns fixed. Like in ASME, there is simultaneous requirement rule in ISO (defined in clause 4.4 of ISO 5458:1998). Its application is a little bit limited in comparison to ASME, but will work fine in your case. It says that: If two or more groups of features are shown on the same axis, they shall be considered to be a single pattern when they are not related to a datum or they are related to the same datum or datum system (datums in the same order of precedence or under the same material conditions) unless otherwise stated."

5. Selection of proper geometrical control depends on how precise you want the sides to be. The hierarchy of accuracy is following (starting from the least accurate): perpendicularity, flatness, roughness. Even all three can be specified on the print. You just have to remember that roughness value shall not be greater than flatness, and flatness shall not be greater than perpendicularity tolerance. If you think perpendicularity is not sufficient control to satisfy you requirements, add flatness. If flatness is not enough, add roughness. As for roughness values, you also have some options depending on how smooth the sides must be.

Hope this helps.

 

[Jieve]

Pmarc,

Once again your help has been invaluable. I am again very appreciative that you have taken the time out to share your knowledge. The drawings I am preparing are for a machine design project that will be used as a learning system at the technical school for which I work. This is the first full project that I have taken from conceptualization to a fully functioning (hopefully) finished product. Now that the parts for the prototype are in production, I have been having a lot of discussions with our machinists, and it is really important to me to provide them with drawings that are correct, professional and ensure proper fit and function of the parts. Thanks to you, I'm making good headway

While I hope I'm not overstaying my welcome here, I do have a couple more GD&T questions before I take a break for the next few days.

1) I have a thin rectangular plate which has a complex series of ribs on the underside and holes and slots through it. The machinists have asked me to dimension everything from one corner of the part as they will be machining the part on one of their "ultra-precise" multiaxis (5 I think) CNC machines, so I have used an ordinate dimensioning scheme and a hole table on the drawing. If I assign datums to the flat face and two sides, is there a way to apply a position feature control frame to all of the holes at once with relation to those datums? Normally this would be done under the leader for the hole callout, but in my case the hole callout isn't there.

2) The more I think about the position refinement control using one position control under another, I feel like I'm starting confuse myself. Assume I have a 4 hole pattern in a square shape on a flat plate, where the flat face is primary datum A and the sides are datums B & C. For argument's sake, I specify a general 0.5mm diameter position control of the holes relative to A|B|C. Then I refine the tolerance, giving it 0.1mm relative to datums A|B. As a result, I am envisioning that the tolerance zone with respect to B is now 0.1mm and with respect to C 0.5mm, giving me somewhat of an oval tolerance zone. In my mind, this only requires that the centerline of the holes be within that oval zone, and does not require them to move together as a group.

However, in the book I have been referencing, it shows a nice graphic of the same exact condition, claiming that the smaller 0.1mm tolerance zones can only move together and their centers are locked at the basic dimensions from each other and to datum B due to the refinement frame. What exactly is locking these refined tolerance zones together? Is it the fact that the original frame is under a 4x dimension callout? Or is it the refinement frame by itself that forces them to move together? In other words, why is the oval I am envisioning above incorrect?

3) Along these same lines, let's say I have the same exact hole pattern as in question 2, but each hole is a different size. I want to lock them together in exactly the same way using a refined position control frame. However, since each hole is a different size, I need a different position control frame for each hole, as I understand it. Is there a way to go about doing this, and if so, how?

4) I am sometimes slightly confused when specifying a perpendicularity control, which dimension is actually being referred to under the general tolerances in ISO 2768-2. Assume that I have a cylindrical part 100mm long and 20mm in diameter with a flat end. I could specify that the cylindrical axis is perpendicular to the flat face, or I could specify that the face be perpendicular to the cylindrical axis. In each case, for the same angle, the tolerance specified in the feature control frame would be completely different. The axis tolerance would be much larger than the face tolerance, as the face "length" is much smaller. I assume the choice as to which feature should be related to which is a matter of datum selection. However, in the general ISO listing for perpendicularity there is a single value (0.4mm (medium class)) for up to 100mm. Depending on which surface I use as the datum, I get either 2.29 degrees (using the value 0.4mm with the face perpendicular to cylinder axis) or 0.229 degrees (using 0.4mm with the cylinder axis perpendicular to the face). The nominal dimension use for the specification is labeled "shorter angle leg". I'm not exactly sure how to interpret that. These numbers are quite different. What is going on here?

5) Finally, this is a somewhat general question, but I find two things somewhat difficult:

a) Trying to combine all of the possible geometric deviations of my parts in a fit to come up with the worst case scenario, and
b) making sure that the tolerances I am specifying are realistic.

Regarding a, I know there is software such as solidworks's TolAnalyst that is supposed to facilitate these calculations while including geometric deviations, but I haven't tried any. These calculations are generally not exceptionally complex for 2 mating parts, but when an assembly has 5 or 6 parts where deviations in the form of different surfaces and features can prevent that assembly from functioning properly, I'm not really sure how to go about this, except to use the envelope principle wherever possible. Any tips?

Regarding b, I am a mechanical engineer but do not have an extensive background in design so I only have a slightly better than rudimentary understanding of what is achievable by certain machining operations. I was just curious if anyone had any tips or charts or something that might help me in this direction.

Thanks!!!

 

[CheckerHater]

Jive,
I am not pmarc, but let me share a piece of my mind:
1) I understand, you are using tabulated dimensions. If you will make your tolerance frames part of your table, they will be well understood, even if this method is not shown in standard book (I don’t have one to look at right now).
2) Datum references in your lower frame override the ones on your upper frame. Your upper frame defines tolerance zones DIA 0.5 fixed in space. Your lower frame defines tolerance zones DIA 0.1 floating together in the direction that is NOT constrained by datum [C]. The centers of your holes have to belong to both sets of tolerance zones TOGETHER at once. So it is not elliptic, but rather moving control.
3) If your tolerance frames will be exactly the same, the “simultaneous requirement” will take care of that. Pmarc explained that in his post.
4) When you rely on ISO 2768-2, your larger feature becomes datum, not the other way around.
5) a) Thick books are written on the topic of tolerance stack-up alone, so it virtually impossible to cover it in the single post (even large one), especially when not seeing actual design. You answered your own question partially when suggested Envelope requirement. I f you are able to keep things wide open, you have greater chances of success.
b) Another larger than life question. Look thru Limits and fits standards. They have examples of typical applications. Then think of your geometric tolerances as refinements of your size. Say, you have shaft with DIA tolerance of 0.10. Straightness of about 80% of it (0.08) would be considered “rough”, 40% (0.04) “medium”, 20% (0.02) “fine”. This is very crude approach, but helps you to not get lost in the jungle that is Engineering.
Good luck!

Sorry pmarc

 

[fsincox]

Pattern tolerance zones must float together or you do not really want a pattern tolerance, but, just separate individual tolerance zones.
Frank

 

[Jieve]

Haha, CheckerHater, Pmarc has been incredibly helpful with his answers to my questions, but of course everyone is welcome to chime in

Thanks fsincox and Checkerhater for the answers!

1) I like the idea of adding the geometric tolerances in the table. Quite clever.

3) About the simultaneous requirement - so how would one implement this on the drawing? Let's say I have my cubic part with the 5 differently sized holes on the same axis. My primary datum is the face the part sits on (perpendicular to the holes), the other two datums two perpendicular faces. If I use a hole position control on one of the holes, being that the combination of holes constitutes a pattern in that they all lie on the same axis, would it then not be necessary to apply position controls to the other holes and assume they are controlled by the same position control? Or does this rule only apply if I were using a second position control refinement frame? In that case, I'm still not exactly sure how I would be sure that it would be interpreted as relating to all of the 5 holes, if it were placed, for example, under the dimension callout 2 x 10mm (for 2 holes of the same 10mm diameter).

4) If the larger feature is the datum, in this case the cylinder, a 0.4mm perpendicularity would result in a 2.3 degree perpendicularity error of the face to the center axis, which seems a bit excessive in that title block angle tolerances are +-1 degree for ISO 2768-m. Seems somewhat strange...

5) I figured these were questions that were a bit too broad to be covered in this post, but thanks for the input. The envelope condition definitely makes things easier, but the fact that a part can still have angle tolerances that cause it to distort at MMC makes this not quite as clean and easy as it first comes across as being.

Thanks!!!

 

[Jieve]

Ahhh, to question 3 - what if i had a group of holes that i wanted to treat as a pattern that do not lie on the same axis? Is there a way to use a position control to specify them as a pattern as in the above mentioned axis rule?

 

[fsincox]

I believe you can use "common zone" in ISO to invoke common patterns.
I have stated in another thread, recently, that I do not believe either system ASME or ISO is attempting to limit the concept of patterns to a single sized feature. I know that it is commonly only shown that way in the books as a simplification of a concept a pattern. The trick is in how you create a definition of a pattern of features that are not actually defined by a single size. Both systems have some provisions for a simultaneous requirement, clearly providing for the concept of a pattern of different types of features. In my work had gear train bearing bores of different sizes that were numbered for section view definition in layout and detailing. We would create a note like: “9X bearing bores (centers numbered #1-#9) to be ……”.
Frank

 

[Jieve]

After doing some research on the CZ ISO specification, it seems that this has been replaced in ISO 14405-1 2010 with CT for "Common Tolerance". If a number of features are to be designated as 1 feature, then a callout with the number of features (5x for example), then CT, then the tolerance control. I have not seen the standard myself, but this is what I have gathered doing some web research. Maybe someone has access to this standard, and can clarify how to actually use this modifier? If any had an example of a drawing using this callout, that wouldn't be too bad either.

Thanks!

 

[pmarc]

Jieve,
CT "modifier" is not a replacement of CZ. Notice that ISO 14405-1:2010 applies to tolerances for linear sizes only. CZ is for common geometrical tolerance zones.
CT's meaning is rather similar to ASME's CF - continous feature modifer.

 

[CheckerHater]

Jeive,
3) To the best of my understanding ISO allows to add notes “simultaneous” and “separate” if condition is not fully clear from the drawing.
4) When you only specify ISO 2768 part 1 as in ”ISO 2768-m” the general tolerance for angles applies. When you also specify ISO 2768 part 2 as in ”ISO 2768-mK” the perpendicularity overrides angle (for features that are shown perpendicular on the drawing, of course).
The reason that “small” perpendicularity allows for “large” angle is that perpendicularity is not angle, like angularity is not angle either. Please look at enclosed picture (left). For two different parts same perpendicularity provides the same fit, which is more important than the same angle.
5) If you want your part not to distort at MMC you have to specify it on the drawing. Like on the enclosed picture (right). This way you have your perfect form at MMC, and as your part “shrinks” away from MMC larger perpendicularity is allowed to fill the gap (in the way shown on the left).

 

[fsincox]

I must admit, I am not pleased to hear that the ISO is undercutting my own arguments, here, on universal communization.
I now have CZ, CF & CT?
pmarc,
Can you say how they are different, please?
Frank

 

[pmarc]

CH,
A short digression:
I fully agree with your statements about point 4) - they are in line with the letter of the standard. However, isn't it a paradox? The same part, fabricated in the same workshop, manufactured in the same process with exactly the same parameters, made of the same material, at the same time can have different perpendicularity error depending on whether part 1 or 2 of ISO 2768 is referenced in a drawing title block. Doesn't it indirectly imply that suddenly workshop accuracy is allowed to change depending on what is shown on a print and not really on their actual manufacturing skills? Isn't it contradictory to the whole concept of general tolerances being based on "customary workshop accuracy"?

 

[CheckerHater]

Pmarc,
Maybe you are over-thinking it.
What you specify on your drawing is not the request to the shop to adjust their “customary accuracy”, but your MINIMAL requirement. The shop has to prove that it is capable of that or better.
You put ISO 2768-m on your drawing. You send drawing to shop capable of producing parts to ISO 2768-kH-E. Who cares? As long as their “customary accuracy” is equal or greater than what you demand, you both are fine.
Or maybe I didn’t understand your question altogether.

 

[pmarc]

CH,
Here is what I mean:
If my minimal requirement for angular tolerance between two features nominally perpendicular to each other (e.g. two adjacent faces of a block) can be covered by ISO 2768-m class, I do not have to specify that tolerance on a print as long as general geometrical tolerances are not needed, right?

But what if for some other reasons those general geometrical tolerances had to be invoked on the print too, for instance ISO 2768-mK, and - like in Jieve's example - general perpendicularity tolerance would allow the tolerance for the angle to be greater than my minimal requirement? What would you do then? I would probably tigthen the angle between faces by placing additional perpendicularity tolerance with a value closely corresponding to the angular tolerance defined by 'm' class.

And now look what happens. According to paragraph A.3.d) of annex A attached to both parts of ISO 2768, saying that: "Those features remaining, which have individually indicated geometrical tolerances, will, for the most part, be those controlling features for which the function requires relatively small tolerances and which therefore may cause special effort in the production", the block now becomes more expensive in terms of manufacturing and inspection, because individual geometrical tolerance has been placed. But is it really a case? No, if only 2768-m was referenced on the print and not 2768-mK. Do you see my point?

 

[CheckerHater]

Pmarc,
I 'm still having hard time to see your point.
First, if shop is capable of producing to 2768-mK, it is capable of producing to 2768-m, so there will be no price increase.
Second, yes. It is your right and responsibility to specify proper control to get the good part.
And that brings us to third (and I am feeling really awkward here): do you honestly prefer plus or minus dimension over geometrical tolerance?
I believe that in any other situation you would suggest using angularity instead of trying to control angle (for obvious reasons). Unfortunately, when it comes to ISO 2768, goal seems to justify the means.
I have to apologize for sounding confrontational. I think discussion is more beneficial then a fight (at least on this forum).
You concern is legitimate as it is in line with the letter of the standard. I agree that in some hypothetical situation it is possible to loosen default angle tolerance. I also cannot believe that responsible designer (including yourself) will control even remotely important feature using plus or minus dimension, not to mention angular plus or minus dimension, not to mention title block tolerance.
So, as a thought experiment-yes. As legitimate real-world concern-not so much.
Still my personal opinion of course.

 

[Jieve]

CH, I understand your point about the tolerances given as being minimums that the shop needs to be able to achieve, and if they can do better with little or no effort they likely will. And I get that the general geometric tolerance -K should refine the -m tolerance, and in this example it's doing the opposite. But coming at this from a less experienced perspective, in light of my perpendicularity example, I interpreted Pmarc's original comment about "customary workshop accuracy" as meaning that if I used the 0.4mm perpendicularity tolerance specified in ISO 2768-2 -K, then depending on the size of the part, I could end up with a part with an axis that is over 92 degrees from the flat face, and that would be considered "customary workshop accuracy". If I chuck the cylindrical surface of this long cylinder in a lathe to cut the flat face, I'm finding it hard to envision ending up with a +-2 degree angle beyond 90 after turning one face flat. If the part were sized slightly differently, say 10mm diameter, the angle would end up as 4.573 degrees. Really?? The face of the part I'm envisioning is no longer looking even closely perpendicular to the axis. But this is also "customary workshop accuracy" based on the standard. Doesn't really make much sense to me, especially considering I've been using some of these values as design guidelines. But maybe I'm missing something.

If I may return to the earlier question about how exactly to use the CZ common tolerance zone to lock together a set of features of different sizes, I have created a drawing illustrating what I was trying to describe before. In the first picture, I have a set of holes. Each hole is individually located to datums A|B|C. The first question I had was rather simple:

1) Is there a better way to indicate that all of these holes, despite their sizes, have the same tolerance zone size without cluttering the drawing with all of the position frames?

In drawing 2 on the second page, I am interested in locking the hole tolerance zones together, as is normally done with a position refinement frame. I have therefore taken what I understood from the above posts and attempted to incorporate it into a drawing. Since the holes are all different sizes, I have used the CZ designation to indicate that they are to be considered a pattern. Then I specified a refinement allowing the smaller tolerance zones of the holes to move around as a group inside the larger zones with respect to datums B & C. Have I done this correctly? If not, could someone correct me?

Thanks!