Profile Tolerance for Slots 2

[Jieve]

Hello Everyone,

I have a flat plate with 5 slots in a linear pattern. Primary Datum A is one face of the plate, and secondary and tertiary datums B&C are 2 perpendicular sides of the plate. I would like to use GD&T to locate and orient the slots. I am not so interested in tightening the distance of the slots from the datums (edges of the plate). I am, however, interested that regardless of where the pattern is, that the slots themselves remain controlled to each other. I would also not like them to be significantly rotated with respect to the plate edges, but translation is ok. If these were holes, is ASME, they could be described using a composite position tolerance from the datums such as:

|Pos|Diam 0.5|A|B|C|
| |Diam 0.1|A|B|

Or as I have learned from this board by the new ISO standard

|Pos|Diam 0.5|A|B|C|
|Pos|Diam 0.1|A|B><|

I’m working to ISO. In this case, however, I am locating slots and not holes. From my research, it seems I can use a surface profile tolerance to locate and orient the slots from the datums. This has brought up a number of questions regarding the use of the profile tolerance.

1) First of all, what would be the best way to achieve what I want to achieve as described above?
2) I have seen a couple of different ways to tolerance slots using GD&T. One was a video from Tec-Ease (ASME) where the callout looked something like:

|Profile|1|
|Pos|Diam 0.5|A|B|C|

I’m not exactly sure what the position is referring to specifically in this feature control frame. Is it referring to the theoretically perfect profile, or a centerpoint, or a centerline? Can this be done in ISO?

3)Other methods which I have seen involved using the profile as a location and orientation and form control, as in:

|Profile|1|A|B|C|

In this case, as I understand it, the slot (assuming we’re talking about a slot) would be located to the datums with basic dimensions and the actual profile could be +0.5 or -0.5 the size of the exact theoretical profile at the exact theoretical location. Therefore, the actual slot would have to be located within these boundaries. Why would one use the method specified in question 2 instead of this method?

4)When using a profile control on a slot, is it necessary to use the all-around symbol on the leader? Is this symbol even available in ISO? I’ve only seen it in the ASME books I have. When is it actually necessary to use this symbol?

5)If a profile tolerance were to be used on a slot to control the form, location and orientation, how would it be measured properly without the use of CMM? Is there a way to do this without very complicated and expensive measuring tools?

Thanks!

 

[SeasonLee]

Would you mind to post a sketch, it will be easier for everybody.

SeasonLee

 

[Jieve]

Ok, here is a pic of the drawing I'm talking about.

 

[SeasonLee]

I am trying to reply all your questions except the first question, I am sure a designer engineer will give you a better suggestions on the 1st question.

2. Before replying your question, let’s start with the basic concept of “Boundary”. When TOP (tolerance of position) callout is used to control the location of elongated holes, it is often done with two tolerance of position controls, one TOP control specifies the tolerance in vertical direction and the second TOP control specifies the horizontal direction tolerance.
If you are using Y14.5M-1994 standard, the word “BOUNDARD” is placed beneath the TOP callout (but not necessary on 2009 standard) to invoke a boundary control. When the word “BOUNDARY” is used,. the tolerance zone is considered to be a boundary control, it’s a virtual condition boundary, there is no axis (or centerpoint , centerline as you mentioned) interpretation, the elongated holes must not violate the tolerance of position boundary, in other words, no portion of the elongated inner surface contour may be permitted to lie within the position boundary.
Take your post #18~#21 elongated pattern hole 9 X 24 as an example, if position callout :
For vertical direction : |POS|1 MMC|A|B|C|
For horizontal direction : |POS|0.5 MMC|A|B|C|
The virtual condition boundary (gage pin dimension) will be 8.5 X 23, no feature surface is allowed to lie within this boundary zone. You may find out more detailed information regarding “BOUNDARY” from Y14.5M-1994 page 143 (or 2009 standard page 126).
I am not quite sure if the “BOUNDARY” is applicable on ISO or not, but the concept of the virtual condition boundary not being violated in ISO standard, since we can easily find out the term MMVC (maximum material virtual condition) in ISO books

3. When the word “BOUNDARY” is used, please don’t forget the MMC or LMC modifier should be specified in the feature control frame. Take your callout and 18~#21 elongated pattern hole 9 X 24 as an example:
|profile|1|A|
|POS|Diam 0.5|A|B|C| should be changed as |POS|0.5 MMC|A|B|C| (no Ø and MMC missed)
The most important is the MMC modifier in the feature control frame, what is the MMC of that feature? You need go to the profile callout first, the default tolerance is bilateral equal distribution, so you have 0.5 tolerance zone on both side of the true profile, for the elongated hole the inward feature is the MMC of the feature, take this MMC feature to calculate the virtual condition.
For |profile|1| callout, the virtual condition is 8 X 23
For |POS|0.5 MMC|A|B|C| callout, the virtual condition is 7.5 X 22.5
When a profile control is used to locate the contour, it will generate two boundary, an inner and an outer boundary, while the MMC positional control creates only one boundary (an inner boundary), this makes the use of a positional control to limit the contour’s movement and location less restrictive than profile, this is the difference between them, perhaps we can consider the position callout here is a refinement of the profile tolerance.

4. There are four methods to denote the amount of coverage of a profile tolerance zone
Leader line touches a surface---this is the default condition
Between symbol---arrow on both end of a line
All around---an circle placed on the bend of leader line
All over---two concentrate circles placed on the bend of leader line
The elongated hole is composed of two semi-circles and two line segments, if the leader line is directed to the upper semi-circle, that means the profile tolerance will apply on this top semi-circle line element only, since the profile tolerance zone covers up to the tangent point at each end of the surface, as soon as the surface changes geometry, the profile tolerance zone ends, this is the default condition for profile. But for the elongated hole, you will control the whole inner contour, so you have to extend the coverage to all around the profile of a given orthographic view, the all around symbol will cover the entire outline of the part in the view shown.
The all around symbol is also used on ISO for sure.

5. A functional gage could be easily built to inspect the part.

SeasonLee

 

[Jieve]

Thanks SeasonLee for the informative response.

Since I am working to ISO and trying not to get confused, can anyone else confirm that what SeasonLee has explained regarding ASME is also applicable to ISO? I was under the impression that the use of english words such as "boundary" was supposed to be avoided in ISO, but I could be completely wrong about this. And the use of the Profile control as described here, is this also done the same way in ISO? Can anyone confirm or comment?

Thanks!

 

[pmarc]

Jieve,
I cannot confirm that what SeasonLee described (use of term BOUNDARY, and the combination of profile + position tolerance) applies in ISO as well. Probably those approaches could work as an extension of principles, but then I would immediately start to prepare for tons of questions from those who are not knowledgeable enough or know enough to ask which ISO standard clearly describes the methods.

My suggestion would be to use profile of surface together with the approach mentioned by you at the beginning of your initial post (i.e. to take advantage of >< modifier). That being said, I am thinking of applying two single segment profile of surface tolerance frames, all around, to both subgroups of 5 slots (tolerance values are exmplary, slots geometry and location are assumed to be defined by basic dimensions. I am also assuming that the refinement you are interested in applies to spacing within 5 holes in each subgroup, but not to spacing between 2 subgroups of slots):
- top tolerance frame - |Prof.|0.5|A|B|C| - controlling location of pattern of 5 slots relative to datums A, B, C;
- bottom tolerance frame - |Prof.|0.2|A|B><| - refining spacing within the pattern of 5 slots, refining perpenducularity of each slot to datum A, refining orientation of slots to datum B, but not their locational relationship to B, controlling form and size of each slot.

 

[pmarc]

SeasonLee,
I have a question to you about your answer to #5. If I understood your reply correctly, a functional gage can be used to verify profile tolerance controlling form, orientation and location of a slot. Am i right? If yes, could you please explain how should this gage look like? What should its size be? Should it be fixed in size or adjustable? Thanks.

 

[SeasonLee]

pmarc

I should say “A functional gage could be easily built to inspect the one constant boundary created by the positional control”. Indeed, if a physical functional gage were to be employed to inspect a profile control, it would be difficult for it to check the boundary created by the profile. Anyway, a functional gage can be accomplished by computer generated models of boundaries and compared against the data collected on parts checked by various means such as computerized CMM, this methodology is in many instances quite capable of inspecting a controlled contour for one or two boundaries, thus making it able to verify either a position or a profile control.

Since we haven’t seen the finalized slots callout, its also hard to talk more detail on the gage design.

SeasonLee