Axis Straightness vs Surface Straightness

[clamschlauder]

I am getting a little confused from trying to learn the applications of both geometric tolerances.

It says here in my textbook that "Perfect form is required at MMC with surface straightness."

Is perfect form not required at all (MMC or LMC) for axis straightness??

In a sample question it states that for axis straightness for a hole the geometric tolerance is only applied at MMC.

For another question it states that for surface straightness on a shaft the geometric tolerance is ignored at MMC because there must be perfect form.

Are there "given" rules that just are what they are regarding this or is there some type of "sense" to follow.

Clarification would be greatly appreciated between these two.

Thanks,

David S

 

[clamschlauder]

As I just saw the section about student posting, yes I am a student but no this is not for a class. I am studying to take my Certified Manufacturing Technician exam.

 

[powerhound]

I don't know how to do the html thing so I'll just put your comments in parenthesis.

You asked: "Is perfect form not required at all (MMC or LMC) for axis straightness?"
Answer: No, this is one way general rule #1 is overridden...by applying a straightness tolerance to a feature of size.

You stated: "In a sample question it states that for axis straightness for a hole the geometric tolerance is only applied at MMC."
Answer: No, you can override rule #1 with a straightness tolerance at MMC or at RFS.

You stated: "For another question it states that for surface straightness on a shaft the geometric tolerance is ignored at MMC because there must be perfect form."
Answer: This is correct because rule #1 says that at MMC, form must be perfect. The exception is a straightness tolerance applied to a feature of size as previously stated.

You asked: "Are there "given" rules that just are what they are regarding this or is there some type of "sense" to follow."
Answer: Yes, there are rules in the ASME GD&T standard. General rule #1 is what these questions are applying to.

Powerhound, GDTP T-0419
Engineering Technician
Inventor 2010
Mastercam X5
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[clamschlauder]

So according to my machinery handbook, RFS is used to indicate that a geometric tolerance or datum reference applies at any increment of size of the feature within its tolerance limits. RFS is the default condition unless MMC or LMC is specified.

If I am reading this correct, the only time perfect form is required is if MMC or LMC is stated (otherwise RFS is assumed). Perfect form would only be required at the stated MMC or LMC. Correct??

I have attached the problem in my workbook that I think is not correct. The book says the answer is (A.) 9.7 mm with this explanation: the 0.3 tolerance only applies when the hole is at its MMC (10.0). Therefore, the pin diameter required to check straightness is 10.0-0.3= 9.7mm

 

[Belanger]

That's right ... 9.7 mm. Notice that this same gage pin would work even if the hole is made at 10.1, 10.2, etc. because at those larger sizes the straightness tolerance is fudged to 0.4, 0.5 etc. (respectively). Thus, the overall combination of size and straightness will always be a constant value of:
actual size - geo tol for that size = 9.7



John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

http://www.gdtseminars.com

 

[clamschlauder]

So how do I know when to override rule #1 and add the tolerance at the hole's MMC, instead of using perfect form at MMC???

If I were to assume perfect form at MMC wouldnt the answer be 10.0mm??

 

[powerhound]

Remember that I said in one of my answers that if you apply a straightness control to a feature of size, the rule that says "perfect form at MMC is overridden." In the case that you have presented, there is a straightness control applied to a feature of size, thus "Perfect form at MMC" does not apply. This has to have covered in your text at some point before you could have arrived at this part of the lesson.

You are calculating virtual condition. The virtual condition of an internal feature of size is it's MMC size minus the geometric tolerance. When you calculate the virtual condition of an external feature of size, you take the MMC value and add the geometric tolerance.

Powerhound, GDTP T-0419
Engineering Technician
Inventor 2010
Mastercam X5
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[clamschlauder]

The textbook I am using is "Fundamentals of Manufacturing" 2nd Ed. It is only supposed to be an overview of many different things, like GD&T. The paragraph that states rule 1 is only 17 lines long spanning 1 paragraph that only covers 1/2 of one side of a normal textbook page. Very General. I cannot find the rule 1 in my Machinery Handbook either.

Also the two problems I stated are from 2 different but similar sources. The one that states perfect form is from the textbook while the one that I sent the picture of is from that same books "workbook."

In another textbook it says this about virtual condition, "When MMC or LMC is specified, virtual condition is used to define the size and shape of the datum feature simulator or the boundary of the tolerance feature surface." What I pull from this is that use virtual condition (meaning MMC - Geom. Tol.) when MMC or LMC is stated.

I guess rereading all of these posts 20 times I think I found where I am getting confused. I will use your answer for an example.

You stated: "For another question it states that for surface straightness on a shaft the geometric tolerance is ignored at MMC because there must be perfect form."
Answer: This is correct because rule #1 says that at MMC, form must be perfect. The exception is a straightness tolerance applied to a feature of size as previously stated.

So in this example, the shaft is not considered a feature of size??

I think I am getting confused with Feature of Size. What I understand about FOS is that it pertains to a feature that is bound by a basic dimension with tolerances. such as a shaft.

I am really sorry if I sound confused and getting anyone frustrated. Not figuring this out is bugging me.

-David Schlaud

 

[powerhound]

You probably need a book that focuses solely on GD&T. A good rule to use to determine is something is a feature of size is the caliper rule. If you can measure it with the od jaws or the id jaws then it is a feature of size. If you must measure it with the depth rod, it is not. One cylindrical surface, such as a pin or a hole, is a feature of size. Two opposed surfaces are also a feature of size but the thing to remember about that is the surfaces must be opposed as in one directly in front of the other. If they are offset from one another then it is not a feature of size.

My suggestion is still to get a book that is focused on GD&T, not one with a slight mention of it because as you now know, it will probably not be sufficient for the more detailed points of the fundamentals.

Powerhound, GDTP T-0419
Engineering Technician
Inventor 2010
Mastercam X5
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[ptruitt]

Getting a book is a good idea. You may want to get one that covers the latest GD&T Standard (ASME Y 14.5 or ISO 1101-2004).

But it is hard to use a book without actually having the Standard that the book is referring to.

Peter Truitt
Minnesota

 

[KENAT]

I would get the relevant version of the standard before you get a book on the subject, but perhaps that's just my preference for going to the source.

Posting guidelines faq731-376

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

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

 

[powerhound]

The reason I think a book is better is because you won't find the phrase "Perfect form at MMC" in the standard and unless you already have a good grasp on GD&T, you won't automatically glean that from the official version of the rule. A good book will explain concepts whereas the standard won't necessarily break it down from the legalese sounding, eye-candy into simpler pieces.

Powerhound, GDTP T-0419
Engineering Technician
Inventor 2010
Mastercam X5
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[clamschlauder]

Thanks guys for all of your help.

What books can anyone recommend to me?

I am still kind of stumped because one question is referring to a shaft and one is referring to a hole, which both are considered a FOS.

The other full question is: What is the size of the geometric tolerance zone for a shaft with a size dimension of dia. 0.625 +-0.005 in and surface straightness of 0.001 in produced at dia. 0.630?

So if I use the rule to determine if it is a feature of size, yes i can put a caliper around a shaft, so it is a feature of size. Right?

The only difference between the two are one is surface straightness and the other is axis straightness.

 

[axym]

David,

The statements in your textbook aren't technically wrong, but the material does seem to be presented in a confusing and misleading way. Some of the terminology relating to features of size and Straightness tolerances in the Y14.5 standard is also confusing in itself. I applaud your efforts to make sense of it all. Here are some clarifications that might help.

Feature of Size: a type of feature that has a size dimension and directly opposed points (inner or outer cylinder, slot or slab, inner or outer sphere). The "caliper test" that powerhound mentioned is a rule of thumb for determining whether or not a feature is a feature of size.

Rule #1: This is a default rule in Y14.5 that applies to size tolerances. The size tolerance itself controls the local cross-sectional size of the feature within the specified limits. Rule #1 adds an additional requirement, that the feature must also conform to a perfect "envelope" or boundary of a certain size. The size of the boundary is the MMC size limit, from the size tolerance. For a cylindrical hole with a size tolerance, the Rule #1 boundary would be a perfect cylinder of MMC size. This is usually checked with a gage pin. By requiring that the feature conforms to the boundary as well as the local cross-sectional size limits, Rule #1 indirectly controls the amount of form error that the feature could have.

Perfect Form at MMC: Rule #1 is often paraphrased as "perfect form at MMC". This is not a rule, it is a consequence of the Rule #1 boundary requirement. It just means that if the feature was produced "at MMC", meaning that its local cross-sectional size was at the MMC limit everywhere, the feature would need to have perfect form in order to conform to the Rule #1 boundary. For a cylindrical feature, perfect form would mean that the feature would be perfectly straight and perfectly round.

Surface Straightness: This controls the straightness of individual line elements on the surface of a feature. It can be applied to planar surface, a cylindrical surface, or other types of ruled surfaces. When the textbook says that "perfect form at MMC is required for surface straightness", this just an awkward way of saying that the Rule #1 requirement still applies and is not affected by the surface straightness tolerance.

"Axis Straightness": This controls the straightness of the "derived median line" of a cylindrical feature. The derived median line (DML) is an imaginary curved line drawn through all of the cross-sectional center points of the actual imperfect feature. So the DML would follow the curve or bend of the as-produced surface. The term "axis straightness" is incorrect, even though it is in many GD&T books and even in Y14.5M-1994. In Y14.5, an axis is a perfectly straight line by definition. The standard (and many GD&T books) also refer to DML Straightness as "straightness of a feature of size" or something to that effect. The intent was to distinguish it from Surface Straightness, but this is also somewhat misleading as Surface Straightness can also be applied to a feature of size (a cylindrical surface). So let's use the term DML Straightness from here on in.

The DML Straightness tolerance has a unique property - it overrides the Rule #1 boundary requirement. When Rule #1 is in effect, the feature's DML would have to be perfectly straight if the feature was produced at its MMC size. The DML Straightness tolerance overrides this requirement, and allows the DML to have imperfect form (bent, wavy, etc.) even when the feature's local cross-sectional size is at MMC everywhere. DML Straightness can be referenced at RFS, MMC, or LMC. In most practical applications, referencing it at MMC is the most functional. The MMC reference makes it possible to use a fixed-size gage to check the DML Straightness, as in the #52 example you posted. In that example, the Rule #1 boundary would be a perfect 10.0 diameter cylinder. The DML Straightness tolerance overrides this, and allows the feature to conform to a 10.0 - 0.3 = 9.7 mm boundary instead.

Sorry about the long winded explanation. This is better explained with figures, and there are good ones in the Y14.5 standard and in most GD&T textbooks.

Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca

 

[clamschlauder]

axim,

I appreciate the long winded response. They have figures in the textbook but I could not see the difference.

What I just got from that post is that the reason for overriding the rule is because the geometric tolerance isnt actually called out on the surface. It is referencing the derived median line (axis). Would this be a correct way of looking at this rule in the future??

If that is the case I guess I really dont see the point because the axis is formed from the surface thus being directly linked to the surface features.

-David

 

[axym]

David,

You're close, but let me clarify a couple more things. The DML Straightness tolerance controls the derived median line, which is derived from the surface. The DML is a curve drawn through all the cross-section centers of the imperfect as-produced surface, and is in general not straight. The axis is also derived from the surface, but it is not the same as the DML. The axis is a perfectly straight line drawn through the center of the "actual mating envelope" of the as-produced surface. The actual mating envelope is the perfect inverse feature that just contacts the extremities of the as-produced surface. For a cylindrical hole, the actual mating envelope would be the largest perfect gage pin that just fits through the hole. The hole's axis is the perfectly straight centerline of that gage pin.

So there is a point to the DML Straightness tolerance. One way to look at it is that a DML Straightness tolerance is like a looser alternative to Rule #1. Where Rule #1 results in the requirement of perfect form at MMC, a DML Straightness tolerance allows imperfect form at MMC.

Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca

 

[clamschlauder]

Axym,

All of that makes sense. Sorry in my last post, last sentence I mean to say DML, not axis. Anyways I totally get what you are saying.

How do computers (CMM) measure surface straightness vs DML straightness? My thinking says that DML would be calculated by running the CMM probe along the height/depth of the shaft/hole along many spots on the surface creating the DML line, therefore measuring that tolerance.

I guess I am getting a little bit off topic here but I think that if I can picture how each is measured in real life, it might help.

- David