Enforcement of inspecting general profile tolerance 5

[prdave00]

In thread1103-276931 the merits of having a general profile on a print controlling features not critical to the part's function were discussed.

Our company is starting to adopt the practice of specifying a general profile tolerance and add a note to the print stating: ALL UNDIMENSIONED FEATURES SHALL BE MANUFACTURED BASED ON THE 3-D CAD MODEL FILE "_____". ALL UNSPECIFIED DIMENSIONS ARE BASIC ASSUMING [SURFACE PROFILE SYMBOL|.010|A|B|C]. Furthermore on some prints for milled parts stipulate conformance to be checked by a CMM scan at the start/end of the batch and at a tool change. I would argue that the absence of this stipulation makes it only an inspection point at the final QC check.

Our parts are complex requiring 5-axis CNC milling / surfacing and we are also transitioning to injection molding. I'd say 50% of the features are .01 to .125" internal and external radii primarily for cosmetic purposes.

My question has many layers...

(1) How does one ensure the same algorithm / methodology is being used to inspect to the general profile across multiple suppliers? Is there a "rule of thumb" about the minimum number of points to probe on curved versus flat face?

(2) The cosmetic radii and such aren't critical enough in my opinion to need to be checked (and am beginning to doubt they even are in lieu of the supplier focusing in on the large features / surfaces), but I can't say this about all the radii. We could waive the general profile tolerance on some of these radii but (a) the print would be messy where there's a bunch of notation flagging features that can be ignored and (b) it seems to defeat the purpose of a general tolerance if it doesn't imply across the board for non-critical features. Any thoughts?

(3) We're transitioning one milled part to molding, but the injection molder we are using says they won't accept a general tolerance on the print. Their argument is that by having the tolerance they are legally obligated to inspect it and certify to it. They say this gives the customer latitude to reject a batch of parts because there is a flaw (void, sink, etc.) in some parts that would make them nonconforming. Anyone else encountered this? I'm actually surprised our machine shops haven't thrown this argument at us.

I'm starting to convince myself that having a general profile tolerance specification is no better than stating "best effort" based on the CAD model. First off I'm doubtful that our fabricators, as reputable as they are, are actually checking against this specification instead of just relying on the accuracy of their equipment / tooling. Secondly, my experience with our injection molder has made me realize how many loop holes a general tolerance might provide for both the fabricator and customer to get out of a contract. Am I being too cynical here?

My apologies if this topic is covered in past post. If that's the case, I'd appreciate a redirect. The term "profile" in the search engine gets plenty of hits.

 

[MechNorth]

First, unless you designate an inspection requirement for any or every feature there's no requirement to inspect based on the drawing alone. The fabricator must ensure that the part meets the specs; how they do that is up to them. If they know their process capabilities and tooling, and control them adequately, then they may never need to do an actual workpiece inspection, relying instead on SPC alone. Application of GD&T (which, by the way means +/- tolerances on size, rule #1, etc. when Y14.5 is invoked) does not mean that feature / control must be inspected. Thus, application of a general surface profile tolerance does not mean that every feature must be inspected.

1) establish an inspection protocol for each workpiece which details what is to be inspected, the sampling method (# points, elevations, etc.), data filtering method, the sampling rate, and the reporting method (is a whisker diagram ok, max'm deviation from limits, etc.)

2) see the two above, then add "flags" only to what you need inspected, and tie it in to an inspection protocol

3)see the above items, and also get a copy of Y14.8 (2009 or 2010?) as it deals with moulded articles now as well as cstings and forgings. Your supplier's argument is incorrect; nowhere in the standard does it say that invoking any geometric control is an automatic requirement for inspection.

The real problem that you're dealing with ignorance of the standard by those who are pushing back. I can quite assure you that an ever-increasing number of companies are migrating to a general surface profile (aerospace, automotive, defense, electronics, moulding and mould tooling) and doing so successfully when they ensure or mandate training for all involved. The reality is that moving to solid-model based production requires it as an enabling step. You'll get a few nay-sayers here, but a lot more seem to support the methodology.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[prdave00]

Jim,

Thank you so much for the detailed response. In hindsight I was being a bit pig headed. I'll need another day or so to completely soak in your entire response, but wanted to extend my appreciation sooner rather than later.

 

[dingy2]

Having a general profile tolerance on the drawing certainly is easy for the Designer but, of course, does not reflect the function or mating relationship of the part. Do you not feel that your supplier would benefit from knowing the feature's functional requirements? From a control or processing perspective, it is critical that we know how the part fits and functions since we could then control those features on an ongoing basis and with a more robust method.

All dimensions on at least one part will be checked in some manner with each dimension numbered. It will not state the number of points contacted but all will be confirmed. The ISIR (initial sample inspection report) will reflect the dimension, tolerance, dimension number and result but, again, that is on one part only.

You did state that on some drawings, it is specified that all dimensions to be confirmed at the start and end of a run and also at tool changes. Do you realize that this cost of confirming non functional dimensions would be costed into the product increasing your price of your product? Is that what you want - increased costs? Do you not really want just the functional features checked in this manner?

Most contributors of this forum are from the design side and if they are in the training field, they preach default profile and positional tolerancing as the panacea to tolerancing of parts. There is nothing in ASME Y14.5-2009 standard that promotes this concept and your suppliers do not appreciate it. As you noticed, some will not accept it.

Please reflect the functional features in a feature control frame. They will then be controlled in a more robust manner.





Dave D.

http://www.qmsi.ca

 

[MechNorth]

Dave, '09 does, indeed, promote the use of a general surface profile tolerance. Pls refer to 2.1.1.b, 2.1.1.e, 2.1.1.2.b, 3.3.25, 8.2.1, 8.2.1.1 which leads to Fig. 8-8.

Also, many of us that teach are, indeed originally from the design side, where we understand the design intent. Most of the instructors that I know personally (and that's a large number of them) who started on the design side also have a fair bit of experience in the manufacturing and metrology side as well. Again, most of us in that category have practical experience as well as knowledge of real world GD&T, garnered from a variety of industries rather than just one.

Perhaps in your automotive background there was a requirement to inspect a first-off 100%, but that's not the case in all industries (even automotive), nor in most from my experience. Unless otherwise required, most competent companies rely on their basic shop capabilities to produce the bulk of the controls required on a drawing, and will verify only those which are at the tight end of their abilities.

That some suppliers won't accept evolution of GD&T (Y14.5) is to be expected, but your tolerance of their behaviour enables them to continue along that line. I work with a lot of small-to-mid size companies as well as some large ones. One of the questions I ask them (usually more politely phrased) is whether they want to grow the business or stagnate & die. If they want to grow, then they're going to have to be competetive and that means gleaning every bit of value from any technology that they implement, including GD&T. I've had clients who contacted me somewhat later when they were able to enter a new market segment because of their grown capabilities.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[dingy2]

Jim:

So you are saying that if companies do not adapt a default profile tolerances, they will stagnate & die??? I think that is a bit of a stretch.

Now to your references but I will just use a couple.

2.1.1 Application
Tolerances may be expressed as follows:
2.1.1 (b) stated "as a geometric tolerance, as described in Section 5 through 9."

Sure, I agree with 2.1.1.(b) but does that promote the general use of surface profile? I don't thinks so. It also states in 2.1.1 (a) "as direct limits or as tolerance value applied directly to a dimension." I don't think that this promotes a +/- tolerance either.

2.1.1 (b) Specifying on the drawing a general note such as: UNTOLERANCED DIMENSIONS ARE BASIC".

This also makes sense so basic dimensions need not have the rectangular box. Does this promote a default profile of a surface? I don't think so.

I was training a group of Design and Process Engineering personnel in a company recently where no GD&T was applied whatsoever. After the seminar (really training) was over, we reviewed some of their drawings. Could GD&T really assist making their drawings reflect the true design intent? I thought so.

In one drawing, there was a hole that was used during assembly for a thermostat control. I suggested positional at MMC so that they could create an attribute gauge simulating assembly. In another drawing, there was a surface on an angularity plane that needed more control for the product to function well. The default angularity tolerance of +/- 30 minutes was not adequate. I suggested using profile of a surface since it controlled not only the angle, location of the angle but also its flatness. Did I suggest that we use a default profile of a surface and positional tolerance? I'll let you answer that one.

I think figure 3-29 in ASME Y14.5-2009 represents a good application of GD&T with a mix of linear and geometrical tolerancing. There is no default profile of a surface tolerance in this example.

In all your statements, I never did see anything about function and relationship of the features. Is this not the design intent that should be relayed to the supplier?

I am going to suggest that there may be some drawings where a default profile of a surface tolerance could reflect the true design intent while in most cases, it certainly doesn't.

I also have to compliment prdave00 for his concern about suppliers and the inspection criteria where default tolerances are used. Possibly he could contact his Quality department about the supplier's Control Plan. Usually, it requires approval from the Customer perspective.

Dave D.

http://www.qmsi.ca

 

[fcsuper]

Dave,

Applying all dims as basic requires GD&T almost by default in my mind. Having a single profile as the source for control of those basic dims is well within realm of ASME Y14.5 (as shown in figure 8.8). It doesn't need to be in the body of the drawing to apply. We have our ALL OVER profile in the title block with no expressed datums? Why no datums? Because the model itself is the reference from which deviation is allowed. Datums are only employed when we wish to establish a relationship between features tighter than the general tolerance would based on the model.

Matt Lorono
Lorono's SolidWorks Resources & SolidWorks Legion

http://groups.yahoo.com/group/solidworks & http://twitter.com/fcsuper

 

[MechNorth]

Dave, "Design Intent" does not mean that every feature has to have a tight control, just that it needs to be controlled; every feature must be defined and controlled. A general surface profile is just an appropriate and effective means of applying an overall control unless directly overridden by an explicit control on a feature or group thereof. If I can live with a 5mm boundary on most features, that's what I'll specify in the general profile tolerance. It's not terribly different from your preferred +/- tolerance except that it is related to a datum reference frame, and the definition is well developed within the standard, and thus EASIER to understand and defend than a +/- tolerance.

And no, I don't see the word "promote" in the standard at all. The standard does provide a number of references that support the use of a general profile tolerance, but it does not promote it as such. In fact, if you look at the disclaimer (page ii), it appears that they have an overall "non-endorsement" statement. Even Section 1.1 SCOPE indicates "This Standard establishes uniform practices for stating and interpreting dimensioning, tolerancing, and related requirements for use on engineeering drawings and in related documents. ..."

Section 2.1 General - "Note: If a model (digital) is used to define the tolerances of the part, see ASME Y14.41 for additional requirements." From Y14.41 3.1.1.4 "Direct tolerancing methods, as defined in ASME Y14.5M, should only be used to define the size of a feature. Geometric tolerancing is the preferred method." Y14.41 Section 6.2.2 Genral Notes "General notes may include default tolerance(s) for the entire model." Y14.41 Table 8-1 (referenced in a variety of sections) lays out where +/- tolerances are acceptable. Y14.41 Section 10.1 Common Requirements (Geometric Tolerances) "A general note defining a geometric tolerance may be specified. More than one tolerance may be specified."
So, since we are talking about a digital model-based product definition, Y14.5-2009 redirects to Y14.41 for some supplementary requirements, and Y14.41 tells us to use a general geometric tolerance. As the only geometric control (currently) capable of controlling location, orientation, size and form as appropriate, is profile of a surface, the logical extension is the use of a general surface profile as the general tolerance. And, in fact, the use of a general +/- tolerance to control locations would also be invalid per Y14.41.

As for your paraphrasing what I said about stagnation & death, please do me the courtesy of actually reading what I wrote rather than what you hastily misinterpreted. It was not a reference to the general profile tolerance, it was the adoption of modern tools and technologies. More OEMs are now requiring SPC and other means of quality verification rather than 100% inspection, even for the first-off. I challenge anyone to prove that they're doing SPC in a meaningful way without using GD&T. One of the key components of a 6-sigma or lean implementation is the use of GD&T ... again, stagnation would be death to a business. As the market continues to shift, suppliers and even OEMs have to find new markets and often enough even new product lines to exploit ... stagnation is death ... GM, Chrysler and a number of others have discovered that painful truth. Many automotive suppliers now produce more than just traditional automotive components because they faced their demise otherwise...stagnation is death.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[KENAT]

prdave00

Using default surface profile you still have to carefully select the value based on function & taking into account manufacturing capability etc.

Sometimes the primary functional driver for the overalls of a large molded plastic part might might be aesthetics. As such a surface profile of say .25" or something may be appropriate.

Anything that needs a tighter tolerance should be so dimensioned. From a cost/ease of manufacture point of view, anything that can be looser should be so dimensioned. This may mean you still end up with a lot of dimensions on your 'minimally dimensioned drawing' - this does not make it wrong.

Not sure how dingy2 can so definitively state that all dimensions on at least one part will be fully inspected. I've seen plenty of situations where this wasn't true.

On your 3) you need to work with the vendor - or find another one. If your 'general' tolerance is truly based on some 'function' - even if it's aesthetics - then them not agreeing to meet it suggests either you don't want to do business with them, or that your requirement does not fall in their process capability so you can't do business with them on this part.

They are correct that it gives you latitude to reject the parts - that is one of the primary function of any drawing/MBD pack.

Do they refuse any general tolerance, or just one expressed as a profile, or is it just yours is too tight for their liking?

MBD and related topics have been discussed on several occasions, may be worth taking a look.

Posting guidelines faq731-376

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

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

 

[MechNorth]

Kenat, the only item I might disagree with is that the general tolerance should be the loosest tolerance on the drawing. That's what ISO says to do (or more correctly if I recall correctly, it says that the shop's loosest capability is to be used, even if that tolerance is not used on the part, with all others specified), but ASME doesn't give advice either way on this one directly(that I've found). My preference is the most common tolerance on the drawing, to reduce drafting and reading. Max, Min, most common, baseline shop capability ... as long as it's on there.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[KENAT]

MechNorth - I don't think I said to use the loosest, certainly didn't mean to. Like you I'd suggest using the 'most common' and then applying extra tols where tighter or looser makes sense.

Posting guidelines faq731-376

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

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

 

[MechNorth]

Sorry, over-read into your example.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[prdave00]

Jim:

At previous companies, we’d generate engineering drawings and indicate which dimensions were inspection points. To me this is mutually beneficial since it communicates, upfront, to the supplier what features the customer considers critical to the function of the part without driving up the cost for unnecesary inspection or relying on the supplier to decide what is critical. It also puts it out in the open as to what the customer’s expectations are without having to negotiate an inspection protocol before the first part is made.

The principal engineer at my current employer does not agree with this practice. Her argument is that the supplier should treat every dimension as critical and indicating inspection points on the print allows the supplier to ignore the other dimensions. So now we add a general profile tolerance note that applies to all undimensioned features. Does she think the supplier should treat this general dimension with the same criticality and attention as the specific dimensions? I’m actually unsure since her actions does not always reflect her attitude…I’ll get to that later.

So now let’s get back to the injection molding supplier. I folded pretty quickly when they stipulated that the general surface profile would have to go and agreed to remove it – maybe because I didn’t see the value. I had things toleranced down to a couple thou and they didn’t bat an eye so why would I think they’d have problem holding a .010” surface profile tolerance on features that were not critical? Maybe they’re hacks, but their track record over the 5 years I’ve worked with them at 2 different companies indicates otherwise. I guess we could have agreed in writing that the general profile tolerance is not required to be inspected, but then what would be the point of having it on the print if they are never going to verify it? I struggle with your logic that there are other ways for a supplier to verify the part meet specs. If I say a part needs to measure between X and Y, what is more concrete than to prove that it measure between X & Y. Can SPC tell you if the mold was made incorrectly? I would argue no. You’d have to measure a part (or the cavity I guess) to show it complies with the print and then apply SPC to monitor the process after it’s been validated.

The real problem that you're dealing with ignorance of the standard by those who are pushing back

I don’t think the suppliers objection has anything to do with Y14.5 since that standard instructs how to interpret GD&T not enforce what dimensions to measure. I would argue that the purchase order contractually obligates the supplier to supply parts that meet all aspects of the referenced print in lieu of any "exceptions to print" noted, etc. I think that’s what they are afraid of is that by signing on the dotted line we could hold the general profile tolerance against them. I think my colleague might hold it against them.

I really do think this comes down to the finding the right supplier and trusting them. I don’t think my colleague has much trust even in suppliers that she reccomends. However, when push comes to shove (and management is in the room), her standards turn to soup. We have sat down with our contract machine shop and reviewed what dimensions/notes will be inspection and how. The general profile tolerance was not an inspection point in the supplier's proposed inspection protocol and there were no objections from my colleague. So why even have the general profile tolerance if no one cares to check it and just rely on the supplier’s capabilities? If you’ve indentified a supplier for their capabilities and they are going to CNC mill the part based on the nominal CAD geometry, then there is no need for the general surface profile tolerance especially if they can hit much tighter tolerances on other features. It becomes benign at best and a loophole at worst.

By the way, I do have a copy of Y14.8-2009, but there hasn't been enough time in the day to actually read the darn thing. Any sections I should focus on?

Dave:

Thanks for your input and the compliment. The general profile tolerance is in addition to a slew of dimensions controlling features that are critical to the function to the component.

KENAT:

The general profile tolerance basically covers the net shape. Some features that it controls do impact function (like avoiding impingement with mating parts that articulate), but for the most part it is to make sure surfaces are blended and aesthetically pleasing.

 

[dingy2]

prdave00:

General default tolerances must be inspected whether default profile or linear. Most often, they are inspected at sample submission and when new tooling is used (covered by sample submission). There is no sense having a dimension and not having it confirmed. I certainly would have loved to be in attendance to a meeting where someone stated they don't inspect all the dimensions where I would be wearing my Quality consulting hat. Your supplier, in my opinion, is dead wrong.

Other features that have a function and mating relationship must be inspected and controlled on an ongoing basis and, hopefully, the drawing reflects each one. Usually, there is a first off, first of shift and a time cycle in which they are controlled. Sometimes, there also is a last of run where tooling wear may be corrected prior to the next run. Manufacturing and Quality will concentrate on these dimensions. All dimensions with method of control should be itemized in a Control Plan (automotive term) and should be approved by the Customer prior to build.

SPC is certainly a tool that can be used and I have been training in that subject since 1986 but you are correct that 1 part or each cavity per mould must be measured. One could have great statistical capability (Ppk of greater than 1.67) but if the average actual dimension is out of specification, it just means that all the product is also out of spec. Also, SPC applications may not be application to all requirements such as positional to a hole at MMC relative to datum A, B at MMC and C at MMC. Here, an attribute gauge (made correctly) is the best control.

If one was inclined to have default profile of a surface and positional tolerances, please make sure that the default tolerance is larger than any profile or positional tolerance shown on specific features in the feature control frame. Also, specify default positional in RFS and state MINOR DIA in case of thread holes and MAJOR DIA in case of threaded studs. We can now have profile tolerances or positional tolerances at MMC on specific features where there is a function and mating relationship. Gauges will be made for the positional features at MMC and they will be confirmed on an ongoing basis. The RFS positional in the default tolerance will be checked, minimally, at sample submission. We will also confirm the specific profile tolerance on a regular basis with a variable measuring method.

Dave D.

http://www.qmsi.ca

 

[KENAT]

The idea of not having a tolerance for every feature, which prdav00 is what you are proposing, scares the #### out of me.

Maybe you have a great supplier now, who always provides OK parts. What if you change supplier in the future? What if the staff at your supplier change? What if management at your supplier change. What if you supplier changes tooling/process... 'Trust in the supplier' is great for the present time, but a crummy way to plan for the future.

I've seen problems caused on parts with incomplete or poorly done drawings. They were made fine for some time by a certain supplier, or operator at a supplier...

Then for one another reason something changed, suddenly parts - which conformed to the limited detail on the print - no longer worked.

Also, it's not uncommon for initial batches of parts to be done by a lead machinist or equivalent who does excellent work. Then for production, they get given to a less senior guy who doesn't do quite as good work. The first batch works, the second batch doesn't. However, because the drawing was incomplete and you were relying on the 'workmanship. of the machinist you are forced to buy off the parts.

Find a tolerance that meets your requirements - even if as I said they are as 'nebulous' as aesthetically looking the same from one part to another - that is within your vendors process capability. Then in the parts quality plan you can determine that for the first article there is perhaps only limited inspection of this just to validate the process, and that in production there is little or none as dictated by the process capability...

Any geometry that infinite variation away from nominal is not acceptable on should have a tolerance, even if it's a loose one.

Also the idea of indicating which dimensions on a drawing are 'critical' 99% of the time scares the #### out of me.

This implies the others are not critical, which can lead to situations where they aren't met. If the tolerances were correctly selected, this will lead to non functioning parts.

Better is to have 'loose' tolerances well within the process capability except where you really need it. You can then have a quality plan that concentrates on features closer to the limit of process capability.

Posting guidelines faq731-376

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

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

 

[MechNorth]

Good post, Kenat.

PRDave, sounds like your current boss is academic rather than rubber-meets-road. I've lived it enough times that I can empathize. I've taught many bosses how to do aspects of their jobs ... sometimes several times until they got it right. I get the impression that you feel that GD&T=critical, otherwise I can't see why you would feel the need to inspect everything. By the way, my background is in plastic mould making, and I know from very personal experience that most (mold) shops that claim to know GD&T really don't understand the basics, much less the subtleties. You have to live with what is handed to you as far as processes & procedures, but as Kenat suggested, look further into the future and see if that tribal knowledge that you rely on today will be there for very long. In a decent shop, with basic understanding of GD&T, they will understand that the general tolerance (by either method) tells them the worst case that will be accepted, and they select their processes and machinery based on that. A highly capable and self-aware shop will use the most economical means to produce the required tolerances and not default to the tightest their shop can produce. That's where SPC really kicks in beautifully. Some shops now rely on ongoing SPC and setup documentation to qualify parts rather than doing full inspections, though most do still do at least a first-off or equivalent. Sorry, I don't know the specific sections of 14.8; it's one of the standards on my reading list.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[prdave00]

All:

Thanks guys. You all get stars from me for your patience and passion - although I'm a little disappointed in Matt's word count.

Kenat:

Sorry for scaring the ##### out of you. Your point is well taken regarding planning for the future, but here's the rub for me... I specify a general surface profile tolerance. The first batch of parts are verified to meet print (but the features controlled solely by the general profile tolerance are not necessarily part of the verification). A quality control plan is implemented that once again may not include inspecting features controlled by the general profile tolerance, but definitely includes features that are critical to function. The part goes into production and the quality plan is used determine the metrics to monitor process capability. So when does conformance to the general profile tolerance get verified? How would one ever now if it deviates if its never explicitly checked? Please feel free to consider these last 2 questions rhetorical given my next paragraph.

I think I'm sold on a general surface profile tolerance on my prints in addition to the explicitly dimensioned features since having it at least attempts to communicate the customer's expectations and guides the supplier to select the most appropriate fabrication and metrology method(s). However, the idea that you'd put a general dimension on the print just to ignore it in the inspection protocol or quality plan is a bit perplexing to me. I can't see how that's any better then putting critical dimensions on the print from the get go.

 

[MechNorth]

PRDave, maybe think of it like an EPA standard for air quality. Do you verify the air quality every day before stepping outside? Likely not, but when it's a bit smoggy outside, you may go and check the weather network to see what's going on, and then make your decision whether or not to venture forth. Certainly part of the issue you are facing is a question of trust with your supplier(s) whether internal or external. If you have a decent history with them, you likely know what they can do consistently, and can base whether or not everything needs to be verified based on that. I've had suppliers that I didn't trust, and still only verified moderately and fully critical features; do I care really that a chamfer is too large or too small as long as it's not affecting function ... no, so I wouldn't check it. When someone says they're checking all dimensions on the workpiece, I tend to think they're being selective and not doing the full workup of "trivial" features. But then, the designer should be designating what is critical and what isn't by some sort of flag and/or metrology protocol.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[KENAT]

prdave00 - it sounds like the issue is with the quality plan not with the drawing. You don't ignore the general profile. However, if it's been chosen to be well within process capability that minimizes the amount of inspection you'd expect to do. I'm always hesitant about basing inspection primarily around 'critical features' and ignoring 'non critical ones'. To me if the tolerances were selected correctly originally this addresses this situation.

For instance on the chamfers Jim mentions. Do I care if the chamfer is too large or small? Well if I've correctly chosen the tolerance for that chamfer - quite possibly. If the chamfer can be larger or smaller, then I should probably relax the tolerance. Obviously in the real world there are gray areas, since we like to simplify things/minimize the number of dimensions we apply.

For instance, say you apply a chamfer with +-.030" tol all around an edge. Let's assume this is well within process capability. In one area there's a feature close to the edge which drives the max tolerance on this chamfer. Lets say else where on this edge there's a fit issue into a radii onto a mating part which drives the min tolerance. Thing is for a large portion of the edge neither of these conditions apply. Should these other portions be dimensioned separately with a looser tol? I'd argue that since we're well within process capability, it doesn't make sense to go out of my way applying extra tols/dimensions to relax an already achievable tolerance. Now, if somehow there's a mess up and the chamfer away from the important area comes in a bit small or big are you going to accept it? I'd say almost certainly.

Also part of what MechNorth says has merit regarding it being something to fall back on if parts 'just don't seem right' even if they've passed minimal production inspection based on sampling of only select dimensions.

You're assuming the general profile tolerance is always just an overall tol to stop the part deviating grossly deviating from nominal. I'm not sure this is an appropriate assumption.

Posting guidelines faq731-376

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

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

 

[Belanger]

Lots of good comments here! Dave (dingy2), you raise a couple of issues that raise my curiosity.

Your wrote that:
"If one was inclined to have default profile of a surface and positional tolerances, please make sure that the default tolerance is larger than any profile or positional tolerance shown on specific features in the feature control frame."

Why do you say that? If I have a general profile tolerance of 2 mm, and I decide that one particular surface can be within 5 mm, is it true that I should change the default to 5 mm and then put feature control frames on every other surface to hold the 2 mm?

Also, you mentioned that "We can now have profile tolerances or positional tolerances at MMC..." I wonder about profile -- perhaps you mean MMB rather than MMC?



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