How the bonus tolerance which we get by Material conditions are used during manufacturing? 1

[sluzzer]

I understood that providing material condition (MMC or LMC),while giving GD&T, gives extra or bonus tolerance. But how this extra tolerance is used during manufacturing?
For example,
When positioning a hole using Positional tolerance with Maximum material condition, we get extra tolerance for positioning, when the hole size is more (i.e., when it is different from MMC). But during manufacturing, the hole is drilled & after that we are measuring whether the hole dia is at MMC or different. Even if it is different, how the extra tolerance which we get from material condition, can be utilized, because the hole is already drilled???!!

 

[drawoh]

sluzzer,

I really like to show 0 positional error at MMC. When I do this, I show a sloppy maximum diameter. That maximum diameter provides allowances for the feature of size error, and for the positional error. No shop in its right mind will try to fabricate to my minimum diameter.

This tolerance provides the fabricator an error budget, which they can exploit as they please. All I care about is that I get parts within tolerance.

--
JHG

 

[CheckerHater]

Even if it is different, how the extra tolerance which we get from material condition, can be utilized, because the hole is already drilled?

If hole is under MMC you can make it bigger to compensate for positional error. Imagine making holes bigger to allow your part to fit over the gage. (providing that holes are not becoming oversized)

 

[Belanger]

GD&T, position tolerancing, bonus, etc. are not speaking to manufacturing. These things simply tell us what the final requirements for the part are.

That said, there is some use for bonus tolerancing in manufacturing, if you know the accuracy and reliability of the process used. For instance, if you know that a certain machine or process is very accurate for size, but not so much for location, then it might be wise to dial the target size up just a tiny bit (rather than just at the middle of the size range). In this way, you can better live with the machine's erratic accuracy for location, and thus get fewer rejects and save money.

The corollary is this: if you discover that a machined hole is out of position after it's made, you can perhaps rework the hole (ream it open further) and salvage the part.

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

 

[3DDave]

There really is no bonus tolerance. None. It's a bad advertising slogan.

Using MMC creates a link between the size of a feature and the location of a feature, which manufacturing is free to trade off for the best cost operation. If one can make holes precisely but can't locate them well, then go with large holes. If the hole size is sloppy but the location can be exact, go with little holes.

After a hole is drilled, one use for the linking of size to location is, if the center of a hole that is smaller than maximum is too far from where it ought to be, one can calculate how much larger the hole could be while in it's current position to make the hole location acceptable (location and size tied together,) and decide if a hole that size is allowed.

 

[CheckerHater]

Belanger,

If the GD&T is not speaking to manufacturing, why should manufacturing listen to GD&T?

 

[dgallup]

One of the biggest advantages of positional tolerances with MMC is that you can build a simple functional gauge for inspection that will 100% tell you if the part is acceptable or not. Stick the part on the gauge, if it fits the part will work. No messing about with CMM's etc. This is a big savings in both time and scrap.

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

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.

 

[Belanger]

Oh, hi there CH.
Think about it: Often people can listen in to a conversation that isn't directly intended for them, and still gain from it.

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

 

[CheckerHater]

So, GD&T is not intended for manufacturing people. That's what I suspected from the very beginning.

 

[sluzzer]

Thanks everyone for the reply
From everbody's reply, I understood that the bonus tolerance is used for a kind of 'rework'.
I mean, after the hole is drilled, we are checking for its position, if the position is not within the limits, instead of scrapping, we are increasing the hole dia & there by increasing the position tolerance limits & making the part acceptable. Am I right?
So is there any relation between hole (feature) tolerance & positional tolerance, that we should follow?

 

[CheckerHater]

Well, the scope of your question was kind of limited: what GD&T, especially “bonus tolerance” can do AFTER the part is already done. Obviously the only thing left was to re-do the part.

But, if you consider what GD&T is telling you, you could decide on tooling, fixturing, QC procedures, and the entire process. GD&T does not specify the process, but it has encoded information on which features of your part can deviate, how, and for what amount. If you can read this information this gives you more freedom and better chances to make good part.
Like drawoh explained in his post, “zero” positional tolerance doesn’t mean “zero” but rather something different and beneficial to you as manufacturer.

 

[CheckerHater]

The entire book can be written on “relation between hole (feature) tolerance & positional tolerance that we should follow”
There are many sources on-line, you can try this one for example:

http://www.mechsigma.com/

Especially this one:

http://www.mechsigma.com/newsletters/2004_07_Newsletter.pdf

 

[KENAT]

CheckerHater, if you take it to extreme an Engineering drawing isn't really for manufacturing people as it specifies what will be accepted not how to achieve it (at least to 14.5-1994).

sluzzer I don't agree that bonus tolerance is only for 'rework' or passing parts on the hairy edge etc. Used and understood properly it allows manufacturing some freedom to tweak their process to maximize the number of good parts made/ease with which they are made as drawoh, Belanger and CheckerHater have touched upon.

So is there any relation between hole (feature) tolerance & positional tolerance, that we should follow?

In ASME Y14.5M-1994 appendix B gives some calculations that explicitly relate these 2 tolerances. They make certain assumptions but are generally applicable.

Posting guidelines faq731-376

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

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

 

[CheckerHater]

Engineering drawing isn't really for manufacturing people

Ken,
There is no need to take anything to the extreme.
Just tell me who will pick the proper drill / reamer to meet the tolerance, and who will “accept” the part after the hole is finished?

 

[dgallup]

The process engineer picks the drill/reamer/boring bar/hone/EDM electrode/laser etc. to meet the tolerance. The QA engineer picks the appropriate gauging equipment, inspection process, inspection frequency and how to handle non-conforming material.

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

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.

 

[drawoh]

sluzzer,

This post has sort of gotten side-tracked. The side-track is relevant.

When you get your part back, you want to inspect it, pass it, and then use it, successfully. During the manufacturing process, you do not want to pay for unnecessary precision.

When you apply a tolerance to a hole at MMC/MMB, you are showing that the positional tolerance is less critical if the hole is over the minimum size. If a hole is fabricated at minimum size, out of position, there is some capability to enlarge the hole, and meet specification. There was an opportunity to use the large drill the first time around, pass the inspection, and avoid the cost and time of the re-work.k

Note how in the case of how I specify things, there is no opportunity to use the smallest hole. They need to enlarge the hole to get a reasonable positional tolerance.

Perhaps the term "speaks to manufacturing" is unfortunate. The reality is that you should not care how they do it. Your drawing should not provide manufacturing instructions. It should describe the part you will accept and pay for.



--
JHG

 

[sluzzer]

Perhaps the term "speaks to manufacturing" is unfortunate. The reality is that you should not care how they do it. Your drawing should not provide manufacturing instructions. It should describe the part you will accept and pay for.

Just a doubt. Suppose if our drawing should just describe the part we will accept & pay for, then why we need to give Material condition modifier at all? It seems like Material condition modifier aids manufacturing only right? Without Material condition modifier itself our drawings describes what we want, am i right? In that case, if we choose not to use material condition modifier then what problem we will get? is it optional?

 

[Belanger]

Suppose if our drawing should just describe the part we will accept & pay for, then why we need to give Material condition modifier at all? It seems like Material condition modifier aids manufacturing only right?

No. The use of MMC does not aid manufacturing only. (Forgive me, sluzzer, if you were in agreement and were merely posing questions a la the Socratic method.)
If a drawing is to describe the part we will accept & pay for, then it's right up the alley of function/design to say that we'll accept a hole that's more out of position — on the condition that it's a larger hole. That is not a directive of any kind to manufacturing; it's just a statement about the final product.

So I stand by my original post: the use of MMC and its subsequent effect doesn't necessarily speak to manufacturing. But manufacturing knows what is allowed by looking at the drawing, and can then use any method to deliver a good part while saving themselves money along the way.

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

 

[3DDave]

MMC is a tool in setting topology limits; limits set so parts that are within those limits are believed to meet the limits of Step 3, below; they should have nothing to do with manufacturing; Manufacturing should know that QA will reject any parts that are outside the limits and try to produce most of the parts to be within them, on a cost informed basis.


Note the lack of gap between steps 4 and 5, a gap that doesn't include manufacturing. It's not that manufacturing has no place in the process, but steps 6-9 can result in an infinite number of ways that are not reflected or controlled by the drawing; If there was a Star Trek Replicator machine that parts just popped out for free, it would not affect the need for step 5 and would eliminate the need for manufacturing input.


How I envision the flow of information:
1) Task defined
2) Concept defined
3) Stress limits, dynamic limits, kinematic limits, and cost limits defined
**Magical step**
4) Dimensions and tolerances that record the magical conversion of functional limits into topology limits
5) QA/QC designs inspection methods to validate/verify parts are within topology limits
6) QA/QC establishes production limits
7) Production/MEs establish production methods to meet/QC limits
8) Infinite divisions of fixturing and detail process planning
9) Cost estimates from fixturing and detail process planning
10) More efforts - raw materials acquisition, rough cutting, fixture acquisition, tool room setup, machine setup, raw part loading, finished part unloading, deburring, cleaning, surface finishing or heat treat or paint, packaging, shipping, customs, receiving, unpacking, storing, retrieving, assembling, QC, final packing, final shipping, and so on. There's not enough room to include everything. Even if there was I wouldn't type it.

 

[3DDave]

1) Suppose if our drawing should just describe the part we will accept & pay for, then why we need to give Material condition modifier at all?
2) It seems like Material condition modifier aids manufacturing only right?
3) Without Material condition modifier itself our drawings describes what we want, am i right?
4) In that case, if we choose not to use material condition modifier then what problem we will get?
5) is it optional?

(Numbers added as it's a five part single question)

A1) If the part can be made perfectly there is no need for any tolerance. Since MMC is a tolerance modifier, if there is no tolerance there is no need for a tolerance modifier. Remove all tolerances and find a supplier of perfect parts.
A2) The MMC modifier aids procurement. Without the modifier, procurement will find fewer suppliers or the suppliers will charge more to make the parts. It doesn't help the metal worker at all except to determine how likely they are to make an acceptable part.
A3) You should get what is on the drawing. Without the MMC modifier the parts will cost more, be less likely to be made, and will not function better, if the MMC modifier was appropriately used.
A4) The parts can cost more or take longer to get.
A5) Sure. Everything is optional. Except death and taxes.