×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Help Interpreting Drawing

Help Interpreting Drawing

Help Interpreting Drawing

(OP)
I'm looking for an explanation of the feature control frame outlined in red within the attached.

I'll take a stab at the meaning: The position of the axis of the shaft (along the entire length of the shaft) must be within a 1.1 diameter circle after the part is first fixtured relative to datum A and then to datum B.

Is this accurate?

Also, what does the "L" (least material condition) mean as applied to datum B? Does that mean when the inspection fixture is produced, the fixture should be at max material condition (4.52 as drawn)?

Thanks for taking the time!  

RE: Help Interpreting Drawing

I'm having a tough time figuring out the design intent given the LMB modifier. I'm pretty sure the fixture won't work since the hole could be anywhere above LMC value and not even fit onto it.

What the feature control frame is saying is that the axis of the long rod must be located within a 1.1 diameter tolerance zone that is perpendicular to A and centered around B when B is at 4.52. As B gets smaller your cylindrical tolerance zone grows by that amount.

This does not make sense to me since the tolerance is applied to the rod and not the hole that the rod is pressed into. If this tolerance were applied to the hole that the rod is pressed into, then it would make sense.

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

RE: Help Interpreting Drawing

A short answer is that the "L" means you can't use a physical fixture.  This is because the datum is to be taken at LMC, which is the largest inside diameter of 4.52 (that's the LMC, not MMC).   When a fixture is made to that, per specification, then anything less than 4.52 wouldn't fit on the fixture!

But numerically, it means that a part with datum feature B at something smaller than 4.52 will get that much extra when checking the position of the needle/shaft.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
http://www.gdtseminars.com

RE: Help Interpreting Drawing

Chaldaean,
1. As powerhound and J-P said, presence of (L) modifier after datum A reference means that hard fixture cannot work well. Such datum feature simulation can be done using virtual datum simulator, but not physical one.

2. Besides, I think it is quite unclear which feature the dim. 4.50+/-0.02 applies to. Looking at the value, I guess this dimension has nothing to do with the threaded hole, so it is probably diameter of the hole reaching 12.1 depth. But that is only my assumption.

3. Which GD&T standard governs the print? Is it ASME Y14.5 or ISO? I am asking because if ASME, then the straightness callout is simply illegal, i.e. straightness tolerance value cannot be greater than 0.012 - shaft's size tolerance, unless it is stated anywhere on the print that in any manner Rule #1 does not apply. I think it would make much more sense from functional point of view to put this callout right below existing position FCF. This would mean that straightness of derived median line of the shaft (this term is not equal to 'axis' of the shaft!) would be limited. And in this case it could stay at 0.25 because straightness of derived median line overrides Rule #1.

If the print is intended to be according to ISO GD&T, then I have no remarks to the straightness callout.

RE: Help Interpreting Drawing

(OP)
Thanks powerhound, Belanger and pmarc for taking the time to pass along your knowledge; I appreciate it.

We couldn't figure out how the fixture would work if the part were above LMC either. The only thing we can figure is the the needle "hub" is plastic (a bit compliant) to accommodate the 0.04mm tolerance.

The drawing is states that it is "based on an interpretation of ASME T14.5M-1994", so perhaps the straightness callout is illegal, pmarc.

 

RE: Help Interpreting Drawing

Yes, a straightness tolerance value must be less than the size tolerance value, unless Rule #1 is overridden.

But if that needle/shaft is non-rigid, then Rule #1 is automatically nullified, so we can't say right now that it's illegal.  It depends on the flexibility.  See Y14.5M-1994 paragraphs 2.7.1 and 2.7.1.3(b).

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
http://www.gdtseminars.com

RE: Help Interpreting Drawing

The straightness is probably illegal. I'm trying to visualize how this thing is screwed over a 1/4-20 nipple. At least from the perspective of an outsider like me, I don't see how the OD of the needle is dynamically related to the ID counterbore in a way where the LMC modifier proves beneficial. The smaller the 4.50 hole gets, the more it can shift relative to the axis of the needle? It doesn't sound right to me.

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

RE: Help Interpreting Drawing

The straightness needs to be applied to the centerline.  Then Rule #1 is overridden and the tolerance value may be greater than the size tolerance.

----------------------------------------

The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.
 

RE: Help Interpreting Drawing

Quote:

The straightness needs to be applied to the centerline.
I have been under the impression that centerlines are not toleranced, features are.  Are there exceptions that I have yet to learn about?

"Good to know you got shoes to wear when you find the floor." - Robert Hunter
 

RE: Help Interpreting Drawing

Centerlines can have geometric tolerances applied to them.  In this case it totally changes the legality and effect.

----------------------------------------

The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.
 

RE: Help Interpreting Drawing

dgallup:

Centerlines are imaginary lines so could you please give an example of a centerline with an applied geometrical tolerance.  

Dave D.
www.qmsi.ca

RE: Help Interpreting Drawing

Centerlines cannot have geometric tolerances applied to them.

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

RE: Help Interpreting Drawing

Let's make sure that we're all using the same definition of "centerline".

Imaginary entities on the drawing, such as centerlines or centerplanes, should not be toleranced or specified as datum features.  These entities are not clearly defined on the actual part.

Certain derived entities representing the center geometry of the actual part can be toleranced.  These might be loosely described as centerlines, but have specific names and definitions.  When Straightness is applied to a feature of size, the Derived Median Line (locus of cross sectional centers) is controlled.  When Position is applied to a cylindrical feature, the axis (perfectly straight centerline of the Actual Mating Envelope) is controlled.

Evan Janeshewski

Axymetrix Quality Engineering Inc.
www.axymetrix.ca

RE: Help Interpreting Drawing

I was speaking strictly in terms of what was originally proposed...a geometric tolerance cannot be applied to a centerline. As in, the arrow points to the centerline on the drawing. I was not talking about a centerline derived from a feature such as the examples you gave.

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

RE: Help Interpreting Drawing

I agree with you on this one powerhound. That is the reason that I asked for an example.  

Dave D.
www.qmsi.ca

RE: Help Interpreting Drawing

Semantics can be important.

"Good to know you got shoes to wear when you find the floor." - Robert Hunter
 

RE: Help Interpreting Drawing

(OP)
To recap from above:

•    The inspection fixture probably wouldn't work (would be too big to fit in the bore if the part was at anything bigger than LMC). The only way the fixture would "fit" is if the hub were plastic and flexed a bit.
•    "As B gets smaller your cylindrical tolerance zone grows by that amount." Or, in other words "with datum feature B at something smaller than 4.52 will get that much extra when checking the position of the needle/shaft."
•    If the shaft is rigid, the 0.25 straightness tolerance on the shaft is illegal as it must be less than 0.12 (the tolerance on the shaft itself). If the shaft is flexible, the straightness is legal per Y14.5M-1994 paragraphs 2.7.1 & 2.7.1.3(b).

Am I missing any additional points or are any of the bulleted points incorrect?

Again, thanks, to all, for your time and wisdom!

RE: Help Interpreting Drawing

I intentionally didn't read any other responses in this thread until I was done typing.  My guess is the L was used based on a fundamental misapplication of Less Material Condition.  The originator likely thought that the tips of the threads (the thru diameter) counted as the less material condition.  Of course LMC doesn't work like that (on several levels).  Though marginally legal, it not practically inspectable and likely produces the exact opposite of what is necessary for design intent.

OK, now I'm going back to read other responses.  Yes to Clakdaean, the B datum actually would vary more in location as material approaches MMC.  I iterate my opinion that L is causing this callout to mean the exact opposite of what I think it intends to mean.

Matt Lorono, CSWP
Product Definition Specialist, DS SolidWorks Corp
Personal sites:
Lorono's SolidWorks Resources & SolidWorks Legion

RE: Help Interpreting Drawing

Quote:

"As B gets smaller your cylindrical tolerance zone grows by that amount." Or, in other words "with datum feature B at something smaller than 4.52 will get that much extra when checking the position of the needle/shaft."
This is not exactly true, I mean the first part of this statement. (L) modifier after B brings datum shift into play, but the datum shift itself does not increase a size of positional tolerance zone - it is always 1.1. When the diameter of datum feature B gets smaller than 4.52 towards 4.48, you have a possibility of moving the part in datum feature simulator B (max 0.04) to fit the toleranced axis of the shaft inside the position tolerance zone. For this particular case the interpretation I am giving now is the same as interpretation given by powerhound, but if geometry was more complicated this wouldn't have to be equal.

Quote:

If the shaft is rigid, the 0.25 straightness tolerance on the shaft is illegal as it must be less than 0.12 (the tolerance on the shaft itself). If the shaft is flexible, the straightness is legal per Y14.5M-1994 paragraphs 2.7.1 & 2.7.1.3(b).
I was not commenting J-P's statement about part's flexibility vs. straightness callout legality before, but in my opinion there is something not OK with this. It cannot be that a drawing reader (inspector, machinist or whoever) is free to interpret such callout depending on part's rigidity. In my opinion there should be a clear indication on a drawing that rule #1 applies to the long shaft or not. A note like PERFECT FORM AT MMC NOT REQD would do the thing if rule #1 is intended to be overriden, otherwise I still think the straightness callout is simply illegal.  

RE: Help Interpreting Drawing

Interesting, pmarc.  I agree that using the "I" modifier or the "perfect form..." note would make it clearer, but paragraph 2.7.1.3 of 1994 says that a non-rigid part subject to distortion after manufacturing forces are removed is automatically exempted from Rule #1.

On an engineering drawing for a rubber band, would I really have to say "perfect form at MMC not required"?   :)

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
http://www.gdtseminars.com

RE: Help Interpreting Drawing

J-P,
Answering shortly to your question, I would say that for clarity such note should be put somewhere on a print.

I know your previous response was directly based on the letter of Y14.5, however in my opinion the standard itself was ('94)/is ('09) not clear enough on this topic and this is why I said there was something not OK with this.

Let me just cite how the newest edition of ISO 8015, dated 2011, is dealing with the subject: "By default, a workpiece shall be considered as having infinite stiffness and all GPS specifications apply in the free state, undeformed by any external forces including the force of gravity. Any additional or other conditions that apply to the workpiece shall be defined in the drawing."  Doesn't this sound much more reasonable?

Let's imagine for a moment that OP's print is according to ISO GD&T. If the shaft/needle was subjected to a form variation in free-state condition, the print would have to say that. Since there is no info about such variation, the feature would have to be assumed infinitely stiff. Now, if this was ASME's rule too, there would be no other choice than unanimous conclusion that for this particular print Rule #1 applies to the shaft and that the straighness callout is illegal.

Apologies if I formulated my thoughts not clear enough.  

RE: Help Interpreting Drawing

Certainly, the position of 8015 is much more clear,  I agree.

If the OP's print is ISO, then we'd assume a rigid part.  However, that's irrelevant to the idea of "perfect form" since ISO does not observe the envelope principle / Rule #1.  (I know you know that, but I'm just musing as I type ... if there's no Rule #1, who cares if it's rigid or non-rigid to begin with?)

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
http://www.gdtseminars.com

RE: Help Interpreting Drawing

Belanger,

ISO does have a couple of conceptional "differences" ::cough::issues::cough:: They do have have rule one when circled E is applied.  Also, up until very recently, the BSI varient of ISO did apply Rule 1 by default, but now uses the Delta D to signify when a drawing is using Rule 1.

Matt Lorono, CSWP
Product Definition Specialist, DS SolidWorks Corp
Personal sites:
Lorono's SolidWorks Resources & SolidWorks Legion

RE: Help Interpreting Drawing

Delta D, not to be confused with the indicator of what changed on drawing revision D.

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

RE: Help Interpreting Drawing

I actually suspect it is just this kind of issue the ISO is tackling by forcing an engineer to "state it if they want it" so to speak, don't just assume that it will happen. It is tougher on us, but I respect the intent and feel it is our job in the end.
I think it is issues like this that show the standards have been too oriented to describing machined solid parts, just like it seems to be too focused on using gages to check things. I understand it is helpful to explain concepts but some seem to think it is the only way to check parts, "because the book shows it that way", how do we little short run shops, ever get by without them? Or should we all just close up shop?
Frank
 

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources