Perpendicularity vs. Title Block Angle Tolerance 2

[Jieve]

Hello,

As I’m continuing to work on drawings for some simple parts and learning GD&T at the same time, I have some more questions for you helpful folks out there.

1)In one application, a short cylindrical spacer sits up against a shaft shoulder. There is a clearance fit 20 E8/g6 at the inner diameter of the spacer to the shaft. I have specified a total axial runout tolerance on the shaft shoulder of 0.1mm. There is a flatness and perpendicularity tolerance respectively of 0.1mm on both faces of the spacer. I have made a 2D drawing of the situation assuming max runout, shaft MMC and spacer MMC to make sure the clearance is still ok. I initially spec’d a perpendicularity tolerance for the hole and tried to work that into the drawing, until I realized that at MMC the parts must have perfect form and that a perpendicularity tolerance on the center hole is therefore unnecessary if the parts fit at MMC (if it is only necessary that they fit). However, I just read that at MMC edge perpendicularity is controlled by the title block angle tolerances (in my case the spacer is 5mm thick, so this means +-1 degree by ISO 2768-m). For a cylindrical part, does this angle refer to the axis angular tolerance to the faces, or to ANY line segment at any point (when rotating the part around its axis) where a face meets the hole? In other words, could the inner hole taper due to the fact that at 180 degrees apart from each other both angles of the line segments are 89 degrees? Or can only the AXIS itself be off by +-1 degree if not specifying a perpendicularity control? Btw. the outer diameter of the spacer has a total runout tolerance of 0.1mm, if this is important to the question.

2)Can anyone point me to a table somewhere with reasonably attainable tolerances within normal shop parameters for different geometric controls? I’m working from the ISO 1101 standard which has a table for fine, medium, course and very course guidelines for straightness, flatness, perpendicularity, symmetry and runout, just to keep my design in check, but something with a little more detail might be helpful including different machining processes. I found something like this once, but can’t find it again. I know machinery’s handbook has a table for IT tolerances resulting from different machining processes, but not sure it had something like this for GD&T (don’t have it with me now).

Thanks!

 

[pmarc]

Jieve,
I realize you wanted much more, but before anything I would like to ask you one question. You said: "I have made a 2D drawing of the situation assuming max runout, shaft MMC and spacer MMC to make sure the clearance is still ok." Does that mean you included runout tolerance value in calculation of clearance between shaft outer diameter and inner diameter of spacer or was it to check some other clearance?

BTW: Is there a chance we could see any image of the prints you made, especially of single components? I am pretty sure it will help a lot in the discussion.

Just to be 100% sure, you are working to ISO GD&T (GPS) on this, correct?

 

[Jieve]

Hi Pmarc,

Thanks for the answer.

When I said a 2D drawing I just meant a CAD sketch with the min ID of the spacer and max OD of the shaft, assuming the shaft shoulder has 0.1mm total axial runout. In other words, the spacer is slightly angled with regard to the shaft centerline. My original intention was to draw the parts together with the different max geometric deviations to see if they still assemble, and as I am somewhat new to this it seemed to be an easy visual way to do it. Then I realized that at MMC the parts actually need to have perfect form and cannot go beyond these boundaries, which simplifies things. I know there are two different principles, one called the envelope principle (ASME?) and I don't remember the other (ISO?). Most of the books I'm reading are written to the ASME standard but I'm working to ISO GD&T, so differentiating has been a little tricky.

I will post a drawing for scrutiny as soon as I have it finished, but any information beforehand would be really appreciated.

 

[Jieve]

Ok, here is the spacer I was talking about. The side with the fillets butts up against a shaft shoulder. I am wondering if the angular title block tolerance (+-1 degree) is applied separately to every point where datum A meets the hole (90 degrees), or only to the axis itself.

Also, since I am somewhat new to making these drawings, any input regarding improvements or things that are not allowed would be welcome before I give these to our machinists.

 

[Jieve]

Thinking about this a little more, it seems that if the size tolerance does not control the angularity at MMC, then anytime a fit is specified for a circular part, a perpendicularity tolerance would need to be used.

As an example, I have a circular part (essentially a hockey puck) that fits into a round pocket. The puck has a thickness of 9mm +0,-0.020mm and a diameter and fit of 33f7/H8. The max diameter of the puck is 32.975mm. The min diameter of the hole is 33mm. However, as I understand it, at MMC there can still be a +-1 degree (based on ISO 2768-m) angle tolerance. The diameter of any cross section of the puck cannot be more than 32.975mm. However, since both sides could theoretically be off by 1 degree (making it look like a parallelogram in the side view), the TOTAL diameter of the part could end up being 33.132mm (32.975 + 9cos(89deg)). In order to control this, a perpendicularity tolerance would be required.

Am I correct in my thinking here?

 

[pmarc]

Jieve,
As for your sketch, could you also show how the shaft was dimensioned in the area of the spacer?

As for your most recent concern and example, assuming that Envelope Principle is in charge and that both diameters are controlled by perpendiculariy callouts to corresponding primary datum planes, the puck and the pocket will always mate since min size of the hole is always bigger than max size of the puck. To use more standard terms, it is a comparison between worst-case sizes of unrelated actual mating envelopes, UAME, of the features, also called worst-case actual mating sizes. Perpendicularity will not have any influence on that.

Perpendicularity comes into play if you want to make sure that the bottom face of the puck (most likely its primary datum feature) always rests flat on the bottom of the pocket (most likely its primary datum feature). In that case you have to compare sizes of related actual mating envelopes, RAME. These sizes are calculated in following way:
- for puck - its maximum size plus maximum perp. tolerance (in linear units);
- for pocket - its minimum size minus maximum perp. tolerance (in linear units).
If RAME size of the pocket is smaller than RAME size of the puck there is a possibility that you will not have planar contact between bottoms of both parts.

Hope it somehow helps.

 

[fsincox]

First welcome,
It is nice to see more ISO people here.
I would not use runout in clearance situations, myself, as it does not accommodate MMC. I would state the mating condition, many people love runout, if they want to check it that way let them, I will state the mating condition. I also believe you should use a perpendicularity callout on the bore. There are some that do not advocate using it because it is hard to check on short diameters. There seem to be two trains of thought on GD&T they are basically:

1) It is our job to describe the functional mating condition. (What I was taught)
2) Only put on the drawing what you want to be checked, and some think it implies how. (The way GD&T is generally used)

I feel the ASME and ISO standards are attempting to achieve the former. The ISO does have the default implied tolerances that MAY make it so you do not need a separate statement, Company title blocks also sometimes specify default angularity tolerances. In the end, you must look at the actual numbers of your mating parts, when it comes down to it; it is not just a discussion of semantics. Looking at one part is only half the story.
Frank

 

[Jieve]

Pmarc and Fsincox,

Thanks so much for the responses. I will post a picture of the shaft mating area as soon as I finish a drawing of it.

As I had mentioned before in a recent post, GD&T is an area that I am new to and trying to absorb as much info as fast as I can to apply it to my drawings, to make sure my parts fit and function properly. So sometimes my questions may be somewhat primitive sounding or strange in that they may incorporate a mix of standards, but as this board is currently my only source for answers to my questions, I really appreciate the input and corrections.

As I said, I have been reading a mix of ASME and ISO references to get up to speed, which judging by the great debates on this board and elsewhere is probably not the best way, but really my only choice in my situation. Last night after reading these posts I researched the envelope principle in ISO. I had been assuming Rule #1 from ASME applied to my parts up until now but as I am working in ISO, it doesn't.

1) Are the envelope principle and rule #1 essentially the same and I can just specify that the envelope principle applies on my drawings?

If form and size are completely independent at MMC, then it seems to me that this would make sizing the geometric tolerance zones a bit more tricky since you have to consider everything - perpendicularity, parallelism, straightness etc. even at MMC.

2) Is it just common to specify the Envelope principle or are there certain techniques or tricks to ensure that you've considered everything and that your parts will always fit?

As soon as I "realized" (or thought this was true) that rule 1 from ASME applied, it suddenly made things easier since as the designer you really just need to consider part fit at MMC (for interference cases)and if it fits with perfect form, you're done.

Getting back to my question about the puck, here is an excerpt from something I read based on ASME:

"As shown by the part in Fig. 3-20, the perpendicularity between size features is not controlled by the size tolerance. There is a misconception that the corners of a rectangle are perfectly square if the sides are produced at MMC. If no orientation tolerance is specified, perpendicularity is controlled, not by the size tolerance, but by the angularity tolerance. The right angles of the rectangle in Fig. 3-20 may fall between 89◦ and 91◦ as specified by the angular tolerance in the title block."

While I think it was indirectly answered by pmarc, I'm still wanting confirmation as to whether the angular title block tolerance of -+1 degree would have the effect that I described (that even at MMC with the envelope principle applied the part could look like a parallelogram from the side view), meaning that essentially the diameter specification is only for individual cross sections and not for the overall part. This just seems counter-intuitive, since I'm spec'ing a diameter with a fit tolerance, but due to the angular deviations of the sides of the puck, if an extra perpendicularity tolerance is not specified (or even if it is), the OVERALL part doesn't actually have to meet that diameter requirement. Pmarc you've said the parts will fit every time if there is a perpendicularity tolerance, I'm assuming you mean if the perpendicularity tolerance is such that it keeps the right angles of the part such that the puck's boundaries are within the min diameter (33mm) of the hole. If this is the case, since there is always some type of perpendicularity deviation from perfect form, the numbers given by the fits don't describe the whole picture, which could be very deceiving to someone not versed in GD&T.

3) Am I correct about all of this??

More clarifications are very much appreciated, and anyone else please feel free to chime in!!! I wanted to get these drawings out ASAP but my lack of full understanding of some of these concepts is keeping me from finishing them.

 

[fsincox]

The geometric tolerancing standards ISO 1101 & Y14.5 by themselves do not control perpendicularity at MMC or otherwise, this must come from a direct statement or a title block angularity, or additional ISO tolerance specifications (the latter two may be too large to tolerate, thus the need for direct statement).

Yes, "the envelope principle" and "rule #1" are synonymous.

Yes, the part can look like a parallelogram with no perpendicularity specification at all, or as large as the angularity tolerance will allow. The datum reference framework is always made of perfectly perpendicular planes, actual parts are not.
Frank

 

[fsincox]

Yes, you can specify the envelope principle in ISO as a default in the title block; You add a symbol, a capital “E” in a circle, next to the general tolerance specification in the title block. You can add the circle “E” just to a specific dimension only, too, If you do not want to invoke it everywhere.
Yes, it does make the engineer's job easier to have the envelope principle, thus its existence. As you have alluded to, this is one of the issues of disagreement in the standards.
Frank

 

[pmarc]

Jieve,
I have prepared one-page presentation showing what I meant by saying that the puck and the pocket will always mate as long as Rule #1 is in charge and min size of the hole is always greater (or at least equal) than max size of the puck. And that a perpendicularity tolerance (whether expressed by title-block tolerance or by perpendicularity callout) will not have any influence on this particular condition.

As you can imagine, for cases #2 and #3 the bottoms of both parts will not be parallel to each other, so if your intent (apart from simple mate) is to assure the puck always resting flat on the bottom surface of the pocket, you have to analyze whether 2 boundaries defined by collective effect of size and perpendicularity error will work together. And for that reason you must take perpendicularity into your considerations. That is why I gave you some formulas allowing verification of those boundaries, called by ASME as Related Actual Mating Envelope (RAME).

For ISO though (since Rule #1 does not apply), you must know maximum perpendicularity errors on both parts even for assuring simple mate. Without them you can't calculate anything, unless you take general tolerances defined by ISO 2768 into account.

Does this help?

http://files.engineering.com/getfil...2642b1c00a&file=assembly_perpendicularity.pdf

 

[fsincox]

pmarc,
Nice work!

 

[Jieve]

Wow Pmarc! Thanks so much for that! And thanks to fsincox as well for the information! Thanks to you guys I've completed 8 of the drawings I will be giving the machinists tomorrow and will most certainly be back as I continue working on the others. For the mating parts I used the envelope principle added onto the respective dimensions. I found the following link describing its use to be helpful:

http://imtuoradea.ro/auo.fmte/files-2007/TCM_files/Simion_Carmen_1.pdf

Again, thanks so much for all of the useful information, I'm definitely getting a solid grip on the subject and I appreciate it so much!

 

[CheckerHater]

Pmarc,
I am uncomfortable with this statement; I find it misleading.
It is correct that long as Actual Mating Envelope of your hole is larger than AME of your shaft you are fine.
You agree that it is only thru for an individual features of size not related to a datum.
IMHO, you cannot say “perpendicularity tolerance will not have any influence on this particular condition” because it is only true when there is no perpendicularity call-out at all.
As soon as you say “Perpendicularity” the amount of it is subtracted from MMC of your hole and AME is shrinking – no matter ASME or ISO.
Do you need a picture?

 

[pmarc]

CH,
Yes, I do need a picture.

 

[fsincox]

pmarc,
Wouldn't a simple mate (peg inside hole) only require a knowlege of straightness not perpendicularity, or do I misunderstand your concept of simple mate.
Frank

 

[pmarc]

Frank,
For "my" simple mate scenario, only comparison between worst-case sizes of Unrelated Actual Mating Envelopes (UAME) is needed - nothing more (assuming Rule #1 rules). So simple MMC size of peg vs. MMC size of hole comparison needs to be done. And you are right that for this scenario straightness rather than perpendicularity is required, but since Rule #1 is applied, straightness is already indirectly limited.

 

[pmarc]

Ah, now I noticed that you were referring to my statement about ISO. In this case I sustain it since in ISO axis perpendicularity relative to planar datum also limits axis straightness, unless straightness is refined by separate callout.

 

[CheckerHater]

Here is the picture (rather rude).
OP question was “how perpendicularity affects fit?”
I believe that if you cannot rest your primary datum feature, then part doesn’t fit.
So I say the part only fits if you don’t specify perpendicularity.
The key is design intent – HOW exactly you want to “fit” your part.
Let me rephrase it: It is up to you as a designer to specify if you need “simple fit” or “fit with datum”, and if you add geometrical tolerance requirement you face the consequences.

 

[pmarc]

CH,
That is what I have been trying to say and show from very beginning of the discussion. Everything depends on design intent - "simple fit" or "fit with datum". If "simple fit" - perpendicularity for puck & pocket situation does not have to be considered at all (assuming we are in ASME world). If "fit with datum" - perp needs to be taken into account.