Close Window

CLICK FOR ARCHIVES

The Tolerancing Engineer Newsletter - January 2016
...by our client company personnel and James D. Meadows using our ‘GD&T HOTLINE’

Subject: Profile of a Line Questions for you! Part 1



Hi Jim,
I hope everything is going well for you. If you don’t mind, I have a few questions for you regarding profile of a line. In no particular order:
1) In the attached PDF, in which I’ve applied profile of a line to the threads of a screw, what orients and/or locates the cross-sections that generate the line elements/establish tolerance zones? I would assume the datums referenced in feature control frames, do this, no? So taking for example “Scenario 1”, would it be correct in assuming that multiple cross-sections could be taken that all must pass through datum axis A?. If this is true, then how would this control really differ from profile of surface? Take enough cross-sections and you would basically end up generating a boundary/envelope that encompasses the whole part, correct?



2) In “Scenario 2”, in which I’ve added datum C to the feature control frame, it would seem to me that there is now only one possible cross-section that could be located/oriented to datums A, B, and C. Is this correct?

3) If the orientation and/or location of the cross-sections are indeed dictated by the referenced datums, then what’s up with Figure 8.27 in Y14.5-2009, which appears to define the direction of the line elements based on the view in which the profile control is applied? I can’t see anything in the standard which supports this.

Kind Regards,
Joe


Hi, Joe,


Let me start with question 3 first. This figure was born out of a question the Y14.5.1 math committee had about what orients the measurement of straightness of a surface’s line elements. The answer we received from Y14.5 was that it was the plane of the view that the straightness was shown in. We asked, doesn’t that constitute an implied datum. They said, basically, “So what?”. We asked them to allow straightness of surface elements to use datum references. They (Y14.5) said no, and if you want to reference datums, use profile of a line. So, from that history, they interpret this drawing with profile of a line which references A and B, that all of the (straightness) profile tolerance zones consist of two parallel lines 0.07 apart, that are oriented to both A and B. Therefore, all measurements must be taken at that orientation.


Question 1 about the profile of a line used on the thread, unless the “means this” drawing beneath the control is actually part of the part drawing, I would surmise they were trying to control the outside diameter’s highest line element (only) as a continuous curvature. I don’t think they meant the entire surface of the thread and all of its line elements. And I don’t think they meant the radial line elements, because if they did, they should have used a local note, such as EACH RADIAL LINE ELEMENT.
Question 2. If my interpretation given about question 1 is correct, then I don’t think the addition of datum C adds anything to the control.


This is what I think. But it’s been a long day.


I hope this helps.


Jim

 


Subject: Profile of a Line Questions for you! Part 2



Hi Jim,


As always, thanks for your insight. Your email just highlighted the fact that I have a serious lack of understanding what profile of a line means when applied to a revolved part! Would you mind taking a look at the attached PDF? On the top half, I’ve laid out a sample drawing. On the bottom half, I’ve laid out three different “options” of line elements that I think the above profile of line specification could be controlling. Without adding some sort of clarifying note, I’m at a loss as to which “option” would most correctly reflect the drawing specification as I can’t find anything in Y14.5, Y14.5.1, Y14.41, etc. that would help me understand this. If you could lend me your thoughts on this, it would be most appreciated.


Thanks,


Joe


Joe,


Option C is most correct, but because all dimensions on the feature being controlled are basic, I don't see a difference between this and a profile of a surface control. This controls the size and the form of the entire surface.
Hope this helps.


Jim


Hi Jim,


Many thanks for the quick response! Would your answer be any different were larger OD of the part (represented by the basic 1.00 diameter) instead some sort of threaded feature? I ask as many folks assume that when applied to a revolved part, profile of a line automatically assumes that you are trying to control only a single high-point/tangent line element (i.e. “Option A” from my drawing).


Thanks,


Joe


Joe,
That's an interesting question, Joe. Line element profile applies to all line elements of the surface to which the line profile points.


As in straightness of a surface, the view in which it is depicted often helps us decipher which line elements are being controlled (straight lines or circular lines).


On threads, if a basic dimension is only shown dimensioning the outermost diameter, I would assume one was trying to tolerance only the size and shape of that outer diameter with profile. And, in that instance, due to the basic dimension, I would see no difference between profile of a line or profile of a surface.


If the entire form of the thread (all aspects of it) were defined with basic dimension and angles, I would assume, again, that they meant profile of a surface, but for the 3D surface.


Got to start lecturing now. I'm in California.


Hope this helps a bit.


Jim



Subject: Re: Question Related to Projected Tolerance Zone


Dear Professor Meadows,


My name is Ayman. I was involved in conducting a tolerance analysis for one of the components for a project I am involved in and I have been using your book “Tolerance Stack-Up Analysis, 2nd edition” as a reference. Particularly I am trying to understand the analysis you presented on pages 107 & 108 for the projected tolerance zone. You mentioned in this analysis that screws and screw holes will be treated as one, just as though they were shafts. As a consequence to this statement, you used the LMC (.2408) and MMC (.264) of the screw in addition to the positional tolerance (0.014) to determine inner and outer boundaries of the screw mounted in its threaded hole. While this makes perfect sense to me, I followed the same steps to analyze the control frame shown in the attached image.

 



I am having hard time explaining to my colleague how the screw tolerances (LMC and MMC) can determine the inner and outer boundary of the screw in the case of a projected tolerance zone. I was asked to remove the screw contribution from the calculation of the inner and outer boundary for the screw mounted in the screw hole. While removing the screw tolerances did not change the boundary locations significantly, I am not convinced that they should be removed. Can you please help me clarify this matter?


Best Regards,


Ayman


Ayman,
If you visualize the clearance hole passing over the screw (forget about the screw head), the clearance exists between the hole and the body of the outside diameter of the screw. Therefore the MMC and the LMC of either the major diameter of the screw thread, or the ground portion of the screw's body (if it has one) determines the clearance. Also, that clearance is affected by the position tolerance on both the threaded hole that determines the location of the screw, and the clearance hole.


I can't see how anyone would disagree with that. But, people sometimes can be stubborn.


James

James,


Thank you for your clarification. I have a follow-up question to check my understanding if you do not mind.


So for a shoulder screw, the MMC and LMC of the shoulder would be considered in the calculation of the clearance and not the LMC and MMC of the threaded portion. Is this correct?


Thank you in advance for answering my questions.


Best Regards,


Ayman


Ayman,


Yes, that is correct. And the MMC of those would be used to determine the available position tolerance. But don’t forget that once the position tolerance on the threaded hole and the clearance hole are assigned, they will also affect that clearance.


James
 



Subject: Drawing Interpretation question



Note to reader: Some views omitted.


James,
Question on interpretation of BP#46 of attached drawing:


Interpretation #1: Threaded feature is positioned .065 basic from datum C because the basic is given from datum C (datum B used for alignment only)


Interpretation #2: Threaded feature is positioned .097 basic (.162 basic - .065 basic) from datum B because datum B is secondary in control frame (datum B used for alignment and mating – p. 508 of your GDT book).


Your opinion is valued.


Mike


Mike,


The threaded feature is located from both B and C, but in different directions. If B had been referenced after C, then B would only have stemmed the rotational degree of freedom. It's unusual that the B surface is referenced before the C hole, in that, usually when a hole is used as a location datum feature, one uses it to locate in both the X and Y directions. But, in this drawing, B locates in the up and down direction (call it the Y direction) and C locates in the left to right direction (call that X).
Hope this helps.


James Meadows
 



Subject: Drawing Interpretation


James,


I have attached a print. I know it’s not “right”, but I don’t know what to suggest to product development to make it “better”.
I’d like to know about necessary datums? Some background info:


• All features will be printed on EOS (additive manufacturing/3D printing) except for the tabs (which will be machined)
• Primary inspection methods will be CMM (all based on GD&T), hard gaging possibly for position (based on final GD&T), and standard mics/calipers
• Position of the screw holes are important (technically appear in 3 planes, but the print only depicts them in two)
• To add additional clarity, the majority of this part is porous (should that make a difference on which face becomes a datum).

 

One face (C4) will be machined flat (potential datum with flatness callout)?

Sorry to bother you, and thank you in advance! Feel free to show this e-mail.


Katherine


Katherine,


Well, in general, it would be nice to stabilize the part to a datum reference frame. It would be great if the datum features reflected how the part works, but sometimes just stabilizing the part and relating everything to everything else is the best way to go. If the surface at C4 is to be machined flat, then it could, as you suggest, become a datum feature and receive a flatness control. Then, it looks like someone thought datum feature B was important enough to make it a datum feature, so if B is perpendicular to the surface in C4 (and I’m not sure that it is), we could assign it a perpendicularity tolerance back to whatever datum feature we call the surface at C4. Subsequent to that we could make all location dimensions and angles basic dimensions. Then make the sizes of the curved surfaces (that are not datum features) basic dimensions. At that point, we could simply position all holes and profile all angled or curved surfaces to the same datum references, with perhaps the machined surface at C4 as primary and datum feature B as secondary. This would create a simultaneous requirement where all features are measured in one set-up from the datums (after the datum features are qualified as meeting their requirements).

 

This would have the advantage of everything being related to everything else to within the sum of their tolerances to the datums they have in common. Everything is related and everything is measured in one set-up. For the surfaces and holes that are critical to function, the tolerances might have to be tight. For the surfaces and holes that are not critical, perhaps the tolerances can be loose. Geometric tolerances are not more expensive, unless they use tighter tolerances. So, tighter tolerances should only be used when the tolerances that are looser are not working properly. This type of complete control is unambiguous, makes manufacturing aware of the relationship tolerances to be held between all things and lets inspection in on how the part is to be fixtured when measured. Functionality should then be better with every feature’s specificity of tolerance and how it relates to every other feature.


I hope this helps.


Jim
 



Subject: Draft Angle

 

Mr. Meadows,

My name is Anthony. I am the Project Lead for our Product Improvement Program. I received your business card from a colleague as a good resource to reach out to you for a drawing interpretation.


See attached illustrations. There area in question is with regard to Note 10 and the Implied 90 degree.

 


The drawing is for a molded part with a note that references a max allowable
draft angle on an (implied) 90 surfaces, no angular dimension.

The question is, can an implied 90 degree surface that also has a note about max draft angle also include the general tolerances on the drawing associated with angles?

The manufacturer is claiming the draft angle can be the max value per the note, plus the general +/-2 degrees relative to any angular dimension (implied or not) that doesn't have a tolerance. One additional point that I did not mention below which may help for clarification...
The manufacturer is attempting to apply the +/- 2 degrees to Datum C.
Any feedback is much appreciated.

Anthony

Anthony,

I don't see a problem with the way the original drawing is specifying the draft angle. The ASME standard on Castings, Forgings and Molded Parts (ASME Y14.8) states that the drawing must specify the draft angle as +DFT or -DFT or DFT INCLUDED. This can be spelled out or abbreviated. This drawing uses the note and the view to do the same thing. In the view, the draft angle is clearly shown as minus draft and in the note it clearly states that the maximum draft is 3.5 degrees.

I don't know how they could have stated the specification more clearly. The general tolerance note of plus or minus 2 degrees is "UNLESS OTHERWISE SPECIFIED". Since it has been specified as I described in my first paragraph, the general tolerance note does not apply here.

I hope this helps.

James

Close Window

© 1997 - James D. Meadows & Assoc., ALL RIGHTS RESERVED

Site Designed & Maintained by VIRTUAL GOLDMINE