Yes, for the most part the complete loss of knowledge about actual manufacturing is resulting in most “Designers” and “Engineers” simply CYA’ing and dropping tiny tolerances on everything. Then everyone wonders how it’s possible that a plate with four tapped holes cost us $8000 dollars. Well you had a material called out that required a special pour at the foundry, you had a flatness callout that required we send it thru several processes down to a lapping to a mirror finish, you’re heat treat call out was a five step process and then you plated it with gold…
At one point manufacturers would have thrown a flag on this stuff. Today it happens so often that they just do it knowing that it’s going to cost an arm and a leg and knowing that a prox bracket holder is not going to the moon despite being designed like it is.
It’s a vicious cycle. One problem with CAM becoming so accessible is that you now have too many machinists these days who don’t really understand much beyond programming, the same way you now have too many QC techs who can program a CMM, but have never acquired the ability to judge workmanship just from holding a part and running their fingertips over it. The end result is a universal overconfidence in the computer side of the process and a tendency to view tolerances as “tight” or “forgiving” only based on their numerical value, rather than connecting them to the setups and steps needed to achieve them.
So yes, I will sometimes put in a WTF tolerance in order to force a dialogue on the point and get people to think before the machine tool starts running.
How would the designer know how the process varies from nominal? What you’re saying means that the designer needs to know that the process varies symmetrically. How would one convey design intent that says I want 1.00", can go over but do not go under?
1.00" +0.010" -0.000" is certainly not the same as 1.005" ±0.005
In my line, the prevailing school of thought says that process and design intent get discussed with manufacturing and recorded with explication, while numerical tolerancing on dimensions tell the conditions that need to be fulfilled in order to have a functional part, no more and no less. So in my world, the two expressions you give are indeed equivalent.
But my beef with one-sided tolerancing on drawings isn’t about being a preacher for a particular way of thinking/communicating, but rather because it necessitates a ton more offline analysis due to there being no feedback in the 3-D design environment.
From a machinist point of view it is. If you give me a dimensions of 1.00 +/.01 or 1.005 +/-.005, I’m going to shoot for 1.005 in both cases. There are some exceptions to this, say dies where if this was a hole they would shoot for 1.010, because as the punch wears the hole will get smaller.
The only way to get “Closer” to a dimension is by making the tolerance tighter.
Now that being said what do you design for features that are either “MAX” or “MIN”? If I have a .060R “MIN” inner radius, what should I model that too? It can be no smaller than .06 but I don’t care if it’s 2.000 or 200.
All that being said I do not think that not using “Nominal all the time in all situations” is necessary or even good design practice in some cases. I think this is particularly true in situations where you have standard fits and tolerances. If I’m going to call out an H6 fit on a hole I’m not including half the tolerance to the model because the H6 fit is -0/+X. Almost all the tolerances in the ISO system are unidirectional. Many are even +/+ and -/-. This is done this way for the express purpose that most people don’t design to nominal, so that the numbers are rounded.
I can model a 40mm hole and put G7 tolerance on it and it’s +.009mm/+.025mm. I don’t model to 40.017mm for several reason. First you would then have to modify the dim in order to get it to read 40mm in order to get the right fit and second you’re far less likely to screw up when designing around 40mm then you are when you are designing around 40.017. Clean round numbers work best for a number of reasons.
From the programming side, yep, its way easier to work with a model that is nominal, but working toward the nominal from a unilateral is not all that difficult in most cases.
I had a junior engineer that was too arrogant and lazy to avail himself of the machine shop just outside our area. In reviewing one of his models I immediately saw things that just weren’t going to fly. It was a plastic part but it straight sides and sharp corners and was modeled more like a simple machined part. I asked him about the draft and he said “Oh, I’m leaving that up to the mold maker.” Okay, how about the parting line, where will that be? “Oh, I’m leaving that up to the mold maker too.” Uh-huh. Where will the gate go? “What’s that?” I asked if I could use his mouse for a few minutes and then quickly put in some draft, which naturally also determined the parting line. I put in a pocket for the gate and added some radii where it would be. His jaw just dropped and he said “That won’t work with the other parts!” But he quickly realized it was his error in not knowing about these things.
The moral of this story is “You have to understand the process you are inherently specifying or else you are nothing more than a cartoonist.” Okay, a 3-D cartoonist.
Not quite. The first thing any part manufacturer wants to know is: what is scrap and what’s not scrap (i.e. what can be billed for). That’s what the drawing tolerance dictates in unambiguous fashion.
There is room to negotiate after that without needing to make that tolerance tighter. It may be that assembly requires less individual fitting if the actual tends toward limit rather than mid-tolerance, etc. But those are things that really merit detailed discussions covering both the commercial and technical aspects of the doing, and the results of those discussions belong on the work order or PO rather than the drawing.
ISO fits are indeed the usual exception to the “middle of tolerance” rule, although most shops will appreciate it if the ISO fits as well have been moved to middle of tolerance in the models they get for CAM. (There are plenty of macros out there for this.) Even so, I now avoid using/citing them in cases where there isn’t a long-standing historical precedent for a defined use case, such as H7 being a transition fit for a metric dowel pin. A tolerance I choose may be identical to 40G7, but on my drawing it will say 40.025/40.009, and although I generally agree with the “clean round numbers” principle during the designing, the final archived model after the job is finished will have 40.017. It used to be that machinists and designers could immediately visualize the approximate tolerance field based on the designation, and it’s just not that way any more.
You know, in theory, of course, you’re right. But I’m a pretty experienced plastics design guy, and when it’s not really obvious, I do leave it to the mold guys. Especially if there is a core pull or something, and the mating surfaces aren’t called out on a drawing. Generally, I consult with the mold maker and then model the draft explicitly, but as a plastic part designer, I’m not going to tell the molder how to design his mold. There are all sorts of things plastic part designers don’t think about that the mold maker needs to determine:
how to get the part out of the mold.
which side does the part stick to
knit lines on cosmetic surfaces
knife edges in the mold
ejector pins
mold cooling
bubbler pins inserts
Otherwise, I’d be designing collapsing cores for every part because I can. Or overmolds because they’re easy. Or specify structural foam process because it allows me thick walls or one of a couple dozen other mistakes that rookies who don’t think they’re rookies make that a mold designer doesn’t make. He knows which parts are expensive or hard to machine or wear out fast, or a part that’s in this catalogue but not that one.
There’s nothing quite as miserable as removing draft and fillets and then redoing them with the correct scheme.
It’s so easy for a plastics designer to double the cost of the mold just by not knowing that the shrink will pull away from some surfaces but on to others. Or that you might be able to allow a thick section with a bubbler, but is that really possible where you want it?
Don’t throw it over the wall, even if you think you know. Have a conversation with the guy who’s machining, designing, or assembling the mold. You don’t want him telling you how to do sketches, so you don’t tell him how to achieve what the project needs him to achieve. I always talk to the molder if I have the opportunity. It makes him happy, it makes you happy that he doesn’t have to come back to you, and it makes your boss happy that the work is only done once.
I’m just going to have to disagree here. Either the print or the model is the master, end of story. Is there “Room for negotiation”, sure, always is. But what that negotiation tells me is that who ever designed the product didn’t design and dimension it properly. If you put +/-.010 on the print and “it will work” at +/-.020…then +/-.02 should have been on the print because that meets the functional need of the part.
That being said there are PLENTY of sectors where there is next to zero "Room for negotiation. I’ve worked on a number of aerospace projects where even if there was something discovered on the print that was patently ridiculous you had to meet the spec. Getting the print changed took an act of congress and if your inspection report did not show that the part met 100% of the specification the part was scrapped, rejected or sent back to you for rework. On some rare occasions you could submit deviations but often those were rejected as well and always went against your supplier record. Ask for too many and you’re out the door.
I’m just not a believer that somehow prints are “Suggestions” and that the true need for the part is determined by purchasing and manufacturing. I think this is simply the lazy mentality created by a severe lack of talented designers that have a solid grasp on tolerances and manufacturing processes. If I’m lazily putting “Negotiable” tolerance on the parts that is unquestionably costing the company money because many, most even, wont come back to “Negotiate”. Most will quote it at what it takes to meet the tolerance on the print.
For the most part I agree. Design to nominal. However I think to say that somehow not designing to nominal is “Wrong” and should never be done leaves out a whole bunch of times and reasons where not designing to nominal is not only not wrong but prefered.
Matt, consulting with the actual process owner, the mold maker in this case, is exactly the point. Thank you for elucidating! (Word of the day there?) Unless we are the “owner” of the process, unless we are the ones that will actually execute the manufacture of the part, there is always someone more knowledgeable.
I had/have a statement above the title block in the last companies where I ran the engineering departments and now with my own consulting: “The vendor is encouraged to suggest ways to improve the manufacturability of this part. Please contact the Engineering Department at (my direct number) with your requests/suggestions.” I made sure we fully considered the manufacturing capabilities/limitations and we rarely had any vendor contact us, however, they often would bring that statement up in our meetings and how much they appreciated it.
I liked to sit down with my vendors, especially ones that were not close to us and we weren’t as well versed as with others. I would ask them these questions:
What is run-of-the-mill that you are doing for others that we are not taking advantage of?
What are more advanced things that you are doing?
What is the state of the art in your industry and where are you with respect to it?
Of course these are very open questions, but it went a long way to building a great relationship and rapidly advancing our achievements. I had one particular conversation with the president and his head of engineering for a powdered metal company. When I was asking these questions on the last one I modified it a bit: “What is the state of the art in your industry and where are you with respect to it? And if you really want to make my day you can tell me you have side-action P/M.” I was sitting next to the head of engineering and across from the president who said, “Dennis, the reason Adam is smiling so big is because he’s about to make your day!” It was an exciting meeting because we were among the first to take advantage of this very new and very beneficial technique. And that came from our investing in learning about what was possible and striving for legitimate ways to achieve more. That process inherently evolved our vendor base.
With all our parts we routinely review them with our preferred vendors prior to release. Most of the time they do not have any big changes to recommend, but we all come out with a lot more peace of mind. However, there are those times when they point something out that is a big improvement and EVERYONE is happy. Usually the big suggestions are either for utilizing techniques that are new to the industry or new to their shop, or the suggestions are from a Design For Manufacturability/Assembly (DFMA) perspective that we overlooked. It’s a win-win.
Dirty Harry has it right: “A man’s got to know his limitations.”
Most of the products I design require some hand-fitting (alignment of optical elements, etc.) during assembly, and how much fitting effort is acceptable, is ultimately decided at some upper business level. What I need to specify as a designer is is the deviation extreme beyond which the part cannot function irrespective of the effort put into assembly.
So for example, I know that 1.005" +/-0.005" will work and specify such; and then after discussion and design review with the head of assembly, we say at 1.008", you’ll likely have 1 hour of fitting, and at 1.005", you’ll have 2 hours of fitting, and at 1.002", you’ll have 3 hours of fitting. The client may indeed choose to tighten the drawing tolerance, or choose to pay a premium for parts closer to 1.008", while accepting all parts within the original tolerance – I’ve seen it both ways. That’s not letting purchasing determine the technical requirements, it’s giving the business owner the information needed for an informed financial decision. Component cost is only one part of the mix.
I have seen way too many expensive downstream errors due to one-sided tolerancing not being reflected in 3D – about the same as with overridden dimensions, hence my initial comparison. Ok, design to round numbers (for ISO fits, those are the nominals) is fine, but archive for future work at middle of tolerance. It’s simply clearer for anyone coming afterwards.
What you’re describing is, in my opinion, still part of the design process. “What fits the function” must always include price and that decision should be made at the design phase and not by purchasing or manufacturing. We do the same thing here with every machine we make. Most machines need to be aligned and need some sort of fitting spacers. How big we make them to start with will determine how much material must come off of them, which equals time and money. If I’m fitting a spindle that I know should only be +/-.06 or so off max and I leave 1/2" extra on the spacer “Just to be safe” well then I’ve just wasted a whole lot of money.
What I’m talking about is the continual thing I see where someone blows a dimension and comes to engineering and says “Will this work” and the engineer doesn’t even need to look at anything and says “I’m sure it will”…that shouldn’t happen.
Just curious as to what errors you end up seeing? If manufacturing is blowing dimensions because they aren’t paying attention to tolerances, that’s hardly a reason to change ones design practices. On the other hand if someone is designing something where unilateral geometry might cause a problem with the design, one would think that in that case unilateral geometry was an inappropriate choice.
Neither of these are reasons to say "Never use unilateral dimensions, at least in my opinion. There are certainly cases where using unilateral geometry and tolerances are more than appropriate and in fact in some cases doing it another way would at very least end up being more difficult at worst incorrect.
On the other hand there has never been a place that I can think of where manual dimensioning is appropriate or the right thing to do.
I remember a time when I was running machines and a young engineer wanted a plaque engraved with writing .03" deep, +/-.03". The crusty old machinist chucked up his best sharpie, did the sign, then sent it out the door. I laughed my ass off and had a beer with him after work, I learned more about the trade from those chats than I ever did apprenticing.
Agreed. Designers and drafters make mistakes. We are human.
I am the one here who decides who we use for fixture manufacture and machining (not product machining). If a supplier sees a drawing that is missing a dimension or has a tolerance like the one described and just makes a guess and sends me back scrap instead of calling me to let me know that i might have made a mistake…then that supplier will be out of a customer.
If the machinist has to guess about something, then the designer/drafter made a mistake. If the machinist makes a guess AND CONTINUES TO MACHINE THE PART, now the mistake is squarely on the shoulders of the machinist. He should have called.
