Profile of a Surface w/ All-Around Modifier and Position question

[Morgama]

Hello Everyone,

I have at least two questions about a drawing that is coming my way soon, possibly more depending on what comes from this. A little background on myself, I've been working as an inspector for about two years now and I think that I have a basic understanding of GD&T, but I'm always learning and trying to understanding things more. A drawing very similar to this came across my desk a few days ago with a question on the GD&T as applied.

I have a couple of questions about what I thought that I knew, one being about the all-around modifier to the profile FCF. Would the modifier, in this case, work to include the cylinders that are protruding from the side of the part. I thought that the profile applied to everything in that view of the drawing, especially with the all around modifier, but am not sure because they are separate features. I look to Y14.5-2009 and see that a profile is an outline made up of one or more features.

8.2 PROFILE
A profile is an outline of a surface, a shape made up
of one or more features, or a two-dimensional element
of one or more features. Profile tolerances are used to
define a tolerance zone to control form or combinations
of size, form, orientation, and location of a feature(s)
relative to a true profile.

I have a colleague who says that the profile would only apply to the block and not to the cylinders.

The second question that I have is regarding the position FCF on the cylinders. It seems to me that they are missing a full 6 DOF constraint, because there is nothing to stop the rotation around the Datum B axis. Is this a compliant callout per Y14.5-2009?

I do have to say that I'm glad to be here, I've lurked for quite awhile and have read many awesome posts relating to questions that I have had in the past. Thanks to anyone wishing to chime in.

~Matt

 

[ewh]

Regarding your second question, datum B is defined as the pattern of 6 holes (as shown, it would actually be the pitch diameters of the inserts), so it does constrain the remaining DOF.

"Know the rules well, so you can break them effectively."
-Dalai Lama XIV

 

[greenimi]

My 2 cents

Short answers for now:
Q1: " Would the modifier, in this case, work to include the cylinders that are protruding from the side of the part." No. If all around profile was intended to take care of the cylinders then the size of the cylinders would be basic .500 not .500±.005 as is currently shown.
The same thing for the length of the cylinders 2.00±.002 shown versus 2.00 basic if all around profile was intended to cover their (cylinder's) length.

Q2: " It seems to me that they are missing a full 6 DOF constraint, because there is nothing to stop the rotation around the Datum B axis. Is this a compliant callout per Y14.5-2009?" Not needed. Simultaneous requirement will take care of the "clocking"
It is compliant: see 4-26/ 2009.

 

[greenimi]

Also make B at MMB to avoid some head ache.

 

[mkcski]

Just an observation:

The periphery (profile) is located from the (6) insert holes - datum B, so wherever the (6) holes "go" the profile and .500 pin follow. Is this the intent?

Certified Sr. GD&T Professional

 

[Morgama]

Thanks for the replies.

To mkcski: I am pretty sure that this is not the intent behind this profile.

To greenimi: With Q2 and simultaneous requirement, is it because I need to look at the outer surface and the pins together as a pattern, that this implies that their basic orientation is controlled? I'm a little fuzzy on this aspect with these being perpendicular features, and not items that are grouped together as is shown in figure 4-39.

Another question that I thought of, when using a profile, must the defining basic dimensions be shown in the view in which the profile is used, or can the basics be contained in other views, or I suppose I'm asking does all the requirements defining the true profile need to be in the view that the profile is called out?

~Matt

 

[AndrewTT]

Consider adding the MMC modifier to the position requirement for the 6X helical inserts. Also consider using the projected tolerance zone modifier. This will ease inspection (see attached excerpt from Meadows text)

 

[greenimi]

Also consider using the projected tolerance zone modifier.

AndrewTT,
Just because I am a little oriented to details.
Your advice is correct but only in some circumstances/conditions: You have to ask the OP/ original post --Matt-- a couple of questions before you draw your conclusion (using the projected tolerance zone modifier) such as: are the screws/threaded studs in place before the assembly? Is the thickness of the mating part greater than or equal to the diameter of the screw/fastener/threaded stud, etc. ?
Then after these questions have been adequately answered a conclusion if the projected tolerance zone need could be made.


Matt,

The tolerance zones are locked together by simultaneous requirement (relationship, pattern, locked by their applicable basic dimensions). I don’t think is matter what is their respective orientations. See fig 7-36/ 2009. Simultaneous requirements still applies for Ø8 and Ø12 holes. Now if Ø12 holes have been 90° from Ø8 holes (not 30°/ would be some holes made into the right face of the part-- so 90° would not been shown--, then simultaneous requirement would still apply.
Am I correct?


As far as the second part of your follow-up question, I am afraid I am not understanding it: All I can say at this moment is that 8.3.1.4 states: “Where a profile tolerance applies all around the true profile of the designated features of the part (IN THE VIEW WHERE IT IS SPECIFIED), the all-around symbol is placed on the leader from the feature control frame.” …”The all-around symbol shall not be applied in an axonometric view on a 2D drawing. Where the requirement is that the tolerance applies all over a part, the all over application is used.”

 

[mkcski]

To mkcski: I am pretty sure that this is not the intent behind this profile.

If that is not the intent, the dimensioning should be revised to reflect what the design "needs". Do you know what the design intent is?

Certified Sr. GD&T Professional

 

[pylfrm]

I have a colleague who says that the profile would only apply to the block and not to the cylinders.

I would say the same thing as your colleague, but unfortunately I can't come up with any solid justification for that.

If all around profile was intended to take care of the cylinders then the size of the cylinders would be basic .500 not .500±.005 as is currently shown.
The same thing for the length of the cylinders 2.00±.002 shown versus 2.00 basic if all around profile was intended to cover their (cylinder's) length.

It seems rather dubious that the dimensioning of a feature would determine whether a separate tolerance applies to that feature. Can you point to any support for this idea in the standard?

Another question that I thought of, when using a profile, must the defining basic dimensions be shown in the view in which the profile is used

There is no such requirement.


pylfrm

 

[Belanger]

Here's an old thread (now closed) that might relate to this all-around discussion?

http://www.eng-tips.com/viewthread.cfm?qid=405001

 

[greenimi]

Quote (greenimi)

If all around profile was intended to take care of the cylinders then the size of the cylinders would be basic .500 not .500±.005 as is currently shown.
The same thing for the length of the cylinders 2.00±.002 shown versus 2.00 basic if all around profile was intended to cover their (cylinder's) length.

It seems rather dubious that the dimensioning of a feature would determine whether a separate tolerance applies to that feature. Can you point to any support for this idea in the standard?

No support from the standard.

I was trying to justify (rationalize) why I am thinking (again my opinion) that the all around profile will NOT include the cylinders.

If the design intent was that the cylinders to be included then, probably, I would use profile with between points to make it clear. (and yes, even the tolerance was the same as the original profile). I would stay away from the all around profile in this particular case.

 

[Morgama]

So I have a few days worth of ideas to answer, thanks everyone.

AndrewTT/Greenimi: I'm not sure what the mating hardware looks like so I can't speak to the need for a projected tolerance zone. I do have a question though on the first statement, I thought that you could not apply an MMC modifier to a threaded hole position because the size of the hole was controlled by the requirements of the threads. Are you able to use the tolerance range of the pitch diameter towards bonus position?

Greenimi: your explanation of the use of a simultaneous requirement does make sense to me.

Mkcski: thinking on it, that actually may be what the designer was thinking, but perhaps could have simplified it quite a bit. What is going on here with this part is that it is a cold plate, a heat sink for a component to sit on. The .500 cylinders are inlet/outlet tubes that will meet with fluid lines and be welded together. What I've heard through the vine is that the designer doesn't really care how the stubs enter this box, what is really important is about the last 0.25in of tube, that will be welded onto another line, is in the right location and orientation.

 

[greenimi]

Matt,

I was suggesting to make B at MMB. In other words the position of the cylinders to be
Position Ø.015(M) to A primary and B (M) secondary.
Also Profile to be .050 to A primary and B(M) secondary.

Regarding position of the 6 holes within Ø.015 (RFS) to A primary, I would say it is correct as long as you belong to that camp of people who are thinking that a straight thread should be called RFS. There is another “school of thought” that is thinking that the correct modifier for straight threads is MMC.
See this thread (and the thread referenced in it) for more info

http://www.eng-tips.com/viewthread.cfm?qid=381644

 

[AndrewTT]

That is a good thread that you referenced, greenimi. I have nothing to add except that I can find examples of position of threads using MMC in 2009 but I did not see any examples of RFS (I know that doesn't mean that you can't do it).

At my work we follow the mantra that MMC is you key to gage-ability and MMB makes the part even more gage friendly. With this in mind we use MMC on the position of threaded holes b/c we believe it allows for gaging without spring loaded pins (that we feel would be required by RFS).

 

[3DDave]

"I thought that you could not apply an MMC modifier to a threaded hole position because the size of the hole was controlled by the requirements of the threads. Are you able to use the tolerance range of the pitch diameter towards bonus position?"

You may be confused by Fundamental Rule 1 which says that tolerances aren't used for stock sizes. What this rule means is that if there is an external specification that covers tolerances it is considered to be double-tolerancing to duplicate that tolerance, not that the tolerance does not apply. It does mean that the user has to look up the tolerance in the external specification.

You can use the pitch diameter range towards a bonus tolerance. I have never seen a method that allows genuinely inspecting** a thread to determine a position and it has always been via the use of a thread gage that is a simulator. Precision gage pins at maximum pitch diameter are more available and suitable for MMC/MMB evaluation. Gages suitable for RFS are significantly more expensive and more difficult to use correctly.

**I mean, going in with a microscopic probe to recreate the surface via 10,000 to 100,000 samples to fit spiral surfaces to compare to the ideal screw thread surface. Maybe this is suitable for very large threads, but short cuts are usually used, such as measuring over or between wires or balls.

 

[greenimi]

I can find examples of position of threads using MMC in 2009

Could you, please, provide the figure number? Maybe 7-21, 7-22? Those are projected ones.

Still enough to conclude that the standard “preferred” way to deal with threads is having them at MMC?
(Again, not projected callouts)

I personally do not think so.

 

[Morgama]

3DDave: You have stated better than I did, the idea that I was trying to convey. When I use a Jo-Plug to measure the location of a threaded hole, I have no size reference, and for acceptability of the thread, we use a go/no-go gage, which tells nothing about the actual pitch diameter, so can't pull the data from there.

 

[AndrewTT]

Yes, I was referring to figures 7-21 and 7-22, which both have MMC used with position of threaded holes. Yes both examples have projected tolerance zones. As I believe others have stated this is what allows (or is believed to allow) for the use of a Jo-plug to gage.

I guess the other way you could go about it would be to modify the position FCF, using a note, to apply to the minor diameter of the threads (and not project the tolerance zone). You could now use a straight pin now to gage the position (tolerance zone exists inside the part). You would have to consider the design intent of the threaded hole before using this approach.

 

[mkcski]

Morgama:

I guess the other way you could go about it would be to modify the position FCF, using a note, to apply to the minor diameter of the threads

Regarding the use of "minor diameter" for thread Position as mentioned in the above quote: Remember - the thread is the functional element to the hole. The minor diameter is clearance for the "crests" of engaging fastener. The PD of the threads must coaxial to the minor diameter or the fastener may not engage.

Let me add a little Mfg input to the discussion. If a traditional "straight" tap is used to create the threads, the tap will follow the path of least resistance and the threads will be coaxial to the minor diameter (typically the tap drill hole). However, if a thread-milling process is used, the threads will "follow" the center of the thread mill (typically the center of the machine tool spindle holding the thread mill), which may not be on the same center as the minor diameter. Thus the minor diameter and the PD will not be coaxial. When inspection checks the position of the minor diameter and not the PD of the threads (that's the drawing requirement), the location of the minor diameter may be acceptable, but the fastener will follow the threads and may be in a different and unacceptable location.

There are several other factors that influence the outcome - class of thread fit, processing sequencing, percent of thread height, etc. But this "centering" issue should be evaluated before using Minor Dia to position threads.

Certified Sr. GD&T Professional